Fundamentals

In this section we shall be covering the fundamentals of 3D modeling in Creo.

A thorough understanding of 3D modeling theory will not only allow you to

move more easily onto the next level but will also allow you to move more
easily between different 3D feature based CAD packages.

This degree is enabling you to become technically competent product

designers and as such CAD is an essential skill, as digital processes become
more dominant in industry that skill will become more important. Over the last
10 years CAD software has become more generic and accessible and easier
to use.

Level 1 will take you through modeling with primitives (Extrudes and
Revolves) to modeling forms with non linear forms and changing cross
sections (Sweeps and Blends). It will then look at how we can modify those
forms using Engineering Features (Fillet, Chamfer, Hole and Shell) and
then how we can replicate those forms using Edit Features (Mirror and
Pattern).

Underlying many of these features is a 2D driving sketch. We will look at

how we build a robust sketch which intelligently captures our design intentions
and flexes appropriately as our form developes.

As we are develop a concept in CAD as technically aware designers, we need

to build our model with a formal and robust structure - this may take a little
more time at the outset but will pay huge dividends as the model becomes
more complex and is developed towards a model ready for mass
manufacture.
What is 3D CAD modelling?

Key terms:
2D
3D
Parametric Modelling
Cartesian coordinate system
Features
Sketch based features
Extrude
Revolve
Sweep
Blend

A three dimensional - 3D - model and environment is ‘simulated’ on a two dimensional - 2D -

screen.

Any entity in that 3D space has parameters to describe its position relative to a default point

or relative to another entity. This is ‘Parametric Modelling’.

The three dimensions X, Y and Z [hence 3D] are described using the Cartesian coordinate

system – 0,0,0 – a dimension for X, a dimension for Y and then a dimension for Z.

You will rarely have to interact with these coordinates but you must be aware of this concept.
In the Department, our preferred 3D environment orientation is the XY plane as the floor and

+ve Z up. Creating models as they would sit in 'real life' with respect to this orientation will

simplify the design process - particularly when we start creating assemblies

Models are displayed by default with no perspective – this can make them look distorted

when interpreted by our normal visual perceptive cues. This default setup is to save

processing power on the PC graphics card.

Perspective can be applied to a model at any time and allows you to better visualise how the

model may look in ‘real life’. Creating some simple elements and construction lines and

printing the result in perspective view can also be a useful basis for 2D hand sketching with

correct vanishing points.

Entities in the 3D environment are called features. We start with a base feature, say a cube,

and then develop it by creating further features which either add or subtract volume from the

the base feature – ie. we may subtract a cylindrical shape from our cube to create a hole.

Recognising how your intended design can be broken down into these
‘primitive’ elements is the key to successful CAD modelling.

In main stream CAD packages these primitive are sketch based features, that is, they

generally start with a 2D sketch. This sketch forms the cross section of the feature.
The primary feature creation methods are:

Extrusion: A 2D sketch is developed along a linear path to a specified

distance to create a 3D form.

Revolve: A 2D sketch is rotated around an axis through a specified angular

distance to create a 3D form.
Sweep: A 2D sketch is developed along a non linear path to create a 3D form.

Blend [Loft]: A 3D form is created by ‘blending’ multiple parallel 2D sketches

Feature Matrix

Cross Section or Section or Xsec - the shape you get when you slice a solid

Trajectory - the path through space the section travels to form the solid

Section Trajectory
Extrude Constant Linear
Revolve Constant Circular
Sweep Constant Non Linear
Blend Varying Varying
Design Intent

Consider a bicycle. It has a vertical central plane about which many of its
components are symmetrical. The wheel rims are concentric to the wheel
spindles. The pedal cranks are apposed to each other at 180 degrees. The
wheel axis is parallel to the pedal axis. The pedal spindles must remain
normal [at 90 degrees] to the mid symmetry plane.

These are fixed geometric and dimensional relationships which need to

remain constant even when the other elements, such as the frame
dimensions, change - this is our Design Intent.

Our design intent within a product is captured and controlled through

dimensions from appropriate reference points and through geometric
relationships - parallel, vertical, concentric, etc.

One of the most common intentions in product design is symmetry. This is

easily and robustly captured in parametric CAD modelers.

Symmetry

In Industrial/Product Design so many of the product we design or work with

are symmetrical - one half of the product being a mirror image of the other. In
the design process, models are developed, modified and updated many
times. Having to make a change to one side of the model and then make
identical changes to the other is not an efficient way to work.

If a model is fundamentally symmetrical then this must be captured in the

modeling process. In parametric CAD systems we can automate this process
such that any change to the original side of the model is automatically
reflected in the mirrored side.
Before starting, make sure you.......

Consider the placement of the model relative to the fundamental datum

planes and use one of them as the symmetry plane. Maybe even rename it
as such - CL is a common acronym for centre line which can later be
migrated into engineering drawings.

Create all of the model to one side of the CL plane to the point it becomes
asymmetrical.

Make sure that any features which must have a smooth transition across the
mirror plane are normal to that plane [see discussion in Level 2 > Surfacing
here]

Mirroring the whole model

When you want to mirror the model simply select the model name at the top of
the model tree and then select the mirror function. This feature will then
contain all the geometry in the model tree needed to create a robust image
across the mirror plane.

Change any feature before the mirror feature the the mirrored half changes
accordingly.

Having a known symmetry plane also simplifies the assembly stage.

see Edit Features for full description

Capturing Design Intent in CAD

A major reason for using CAD to design a product is to enable easy

development, dimensions may change many times before a final solution is
agreed upon. If the design intent is efficiently captured in the model and
assembly then development is simpler, quicker and more robust.
Consider the above image. If I was communicating this part to a third party,
part of my description would describe a rectangular pad in the middle of the
angled surface and two holes drilled into the rectangular pad.

The rectangular pad is one element and the holes in the pad are a another.
Each of these elements have their own dimensions to describe them and then
dimensions which place them relative to other elements. My feature
dimensions and feature position relative to parent features.

The pad is placed on the angled face a distance from the side wall and a
distance from the bottom edge. It is then x mm wide and y mm high. If its
position changes I don't want its size to change.

The holes are x mm and y mm from the edges of the pad. If the pad moves
the holes need to stay in the same place on the pad.

These two last statements are my Design Intent. This design intent needs to
be captured in my dimensions.

If I try and move the pad using the dimensions [20 and 10] on the left the pad
will also change size and I will have to change the other dimensions [38 and
45]
The dimensions on the right better capture my design intent and I can move
the pad without effecting its size. But this dimensioning scheme still does not
effectively capture the central positioning of the holes on the pad, ideally the
holes need to be dimensioned around the centre of the pad.

Considering design intent as you model becomes more important as models

become more complex and the consequences of changing one dimension
become more dramatic. Getting into good habits early on will save you time
as your designs become more complex.

Sketching
Key Terms:
Sketchplane
Sketch Orientation
Sketching References
Sketcher
Intent Manager
Design Intent

Curves - entities in a sketch whether they are straight or curved!

Sketch based features

A 2D sketch is developed to create a 3D form

Standalone or Internal Sketch?

The 2D driving sketches for your features can either be; Internal to [embedded within] the
feature - created whilst creating the feature, or, standalone independent features. Some
sketches have to be internal - the section sketch for a sweep for instance.
Internal
For simpler features such as extrude and revolve it is generally quicker and creates a tidier
model tree to create the sketch within the feature. Internal sketches can also be checked
using the Analysis Tools (see end of this page) relative to that feature type.

Start the feature > right click [in the graphics area] > Define Internal Sketch

Independent

Independent sketch features which are selected whilst creating the model feature have a
number of advantages for more complex geometry and feature creation methods such as
sweeps and blends;

You can visualise the form before creating the feature though the 'wireframe' sketches

If the feature fails or is deleted you do not lose the sketches driving the feature.
Setting up the Sketch
When creating most sketched based features there are three common setup consideration
which can be summarised as:

1. Sketchplane

The Sketchplane is the flat plane – surface or datum plane – on which you are going to

draw the 2D driving sketch underlying your feature. Whilst in Sketcher, click on the icon
in the Sketch toolbar to change the sketchplane or orientation.

2. Sketch Orientation

The Sketch Orientation is generally assigned automatically and you can usually skip this
step and accept the reference chosen by the system.

It decides in which of the four possible orientations the ‘four sided’ sketchplane is viewed - like
decided whether you use a piece of paper in landscape or portrait. The sketchplane is
parallel to the screen, there has to be a surface or datum plane which is perpendicular – at 90
degrees – to the sketchplane which can be chosen to face to the right, left, top or bottom.

Sometimes you may want to change the sketchplane orientation. The reason behind this
process is to orientate the coordinate system within the sketch.

There is also a direction arrow which indicates which side of the Sketch Plane you are looking
onto - click the arrow the flip the view direction.

Creating text on a part is an obvious example where the Sketch Plane orientation is very
significant.

3. Sketching References

The position of your sketch on the sketchplane needs to be described with dimensions and
geometric constraints - refer to the previous section on Design Intent. Sketching
References are the entities from which dimensions will start. You will need to decide on
appropriate sketch reference before you start sketching. Click the sketch references icon
to add or change sketching references.

A coordinate system, point or perpendicular axis can be chosen alone and will generate
both vertical and horizontal dimensions. Otherwise choose a vertical and a horizontal
perpendicular plane (surface or datum plane) – edges are not robust references.

Sketcher is the 2D sketching environment in which you will create feature driving sketches or
planar reference curves.

The brown dashed lines are the sketch references. The Sketching References dialogue box

can be returned to add or delete references at any time via the sketch references icon

Constraints

Geometric Constraints

A Sketch is a set of curves which must be Resolved before it can be used to generate a
solid. The Intent Manager constantly resolves the sketch as you add curves to it. To be
resolved, a Sketch must contain enough dimensional and geometric constraints to fully
describe the curves.

As your sketching and the Intent Manager is trying to apply/snap a

particular constraint:

 right click to toggle through lock/disable/enable the

constraint
 use Tab key to toggle active constraint
 press and hold Shift to disable snapping to new constraints

See HERE for expanded explanation of Geometric Constraints

Tangency on Wikipedia - HERE

Dimensional Constraints
Once you have some curves, you've dragged them to the right
proportions and you've added geometric relations then you can add
dimensions - dimensional constraints.

LMB to select the geometry to dimension, MMB to place the

dimension. Place the dimension with MMB in the position you
would draw the dimension on paper.

 LMB to pick a line, MMB to dimension the length of that line

 LMB to pick 2 parallel lines, MMB to dimension the distance
between the lines
 LMB to pick 2 non parallel lines, MMB to dimension the angle
between those lines
 LMB to pick an arc, MMB to dimension the arc radius
 LMB to pick a circle, LMB to pick the circle again, MMB to
dimension the circle diameter
 DO NOT dimension a circle with a radius
 LMB to pick points or centres, MMB to dimension the distance
between those points

Useful dimensions:

In sketcher, select a chain of lines, curves, etc to create a perimeter,

Edit > Tools > Convert to > Perimeter and it'll create a
dimension for the perimeter length.

Arc length: LMB - arc endpoint, arc endpoint, arc. MMB to place
dimn. As below:

Perimeter - dimension reporting the combined length of a closed

loop of curves

Ctrl Select the loop of curves > select an existing dimension on one
of the curve to show the position of the perimeter dimension.

Good Sketching

1. Curves [to scale]

2. Geometric Constraints
3. Create Dimensions
4. Modify Dimensions
Creating a robust and successful sketch as the basis of most of the common ProE features is
a crucial step on the way to a successful model.

Step 1: Use the sketcher grid and zoom in/out to make the graphics area the same size as
your intended sketch.

This will avoid problematic ‘bit by bit’ scaling through modification of dimensions in the sketch
once it is completed. Large movements of entities will often result in extreme distortion of the
sketch.

Step 2: Using Lines and Arcs (rather than trimmed Circles and Squares) starting from one
point and create the sketch in a continuous line.

Trimming circles and squares can often result in end points becoming disconnected so
causing open loops which are hard to solve. You are also more likely to create lines on top of
lines - very hard to track down. Starting from one point and switching from line to arc as you
work around the loop will ensure good connection.

Step 3: Create the sketch to the correct proportions.

This will avoid lots of resizing work. Drag points and entities to approximately reshape the
geometry.

Step 4: Apply geometric constraints.

Connect the sketch to the sketching references and use geometric constraints before
dimensional constraints to fix its shape and proportions. This will minimise the number of
dimensional constraints. The common constraints you will use are Tangency and
Coincidence.

Step 5: Apply dimensional constraints.

It is good practise to try and leave the sketch with no grey, weak dimensions. This ensures all
dimensions have been considered and checked.

Step 6: Modify the dimensions.

Using the pick icon, simply double click a dimension to modify it. Also, using the pick icon you
can drag a box around all of your dimensions to select them and then pick the modify icon to
list all the dimensions for easy modification. Uncheck the regenerate option as this may
cause distortion as each dimension will be updated as you make changes.

Step 7: Resolve sketch failures.

If the sketch fails it is most commonly due to either disconnection between points causing an
open loop – look for weak dimensions of zero – or because you have lines on top of lines –
very hard to find. This last issue is the main advantage to creating the sketched loop an entity
at a time continuing from the end point of the previous entity using line and arc segments

This method of creating robust sketches is by no means the only way, there are always
exceptions everyone develops their own techniques but I have found it to be a good starting
point.

Round up/down your dimensions - do you really want your

part 47.63mm wide or 42.97degs? Remember, these dimensions will
migrate to your engineering drawings.

Interrogating your sketch

For a solid feature your sketch needs to be either;

- a single closed loop

- multiple closed loops which do not overlap

Common issues which cause a sketch to fail are;

Tags

Usually through bad trimming. Look for unexplained dimensions.

Line on line
One line exactly overlapping another is seen as another [incomplete] loop. Usually through
bad trimming. Tricky to find. Look for unexplained dimensions.

Disconnected endpoint

Endpoints seem to join but don't have appropriate constraints. This can happen when using
the copy edge function.

Section Analysis Tools

With both Internal and Independent sketches, the system can use a range of tools to highlight
issues with your sketch.

Introduction to ProEngineer through the Extrude feature

Extrude: A 2D sketch is developed along a linear path to a specified distance to create

a 3D form
The Extrude feature is the most common and simplest of the fundamental feature creation
tools in CAD, it is a common start point in the building blocks which make up your model.

Base features - Extrude, Revolve, Sweep, Blend - can either create or

remove material - See Video HERE

Watch a video on how the use the Extrusion functionality HERE

Graphics area

Most of the control over the feature can be accessed through the graphics area right click
menus, control handles and clicking on arrows.

Remember you have to press and hold the right mouse button to access the right click
menus.

- right click menu to create internal sketch

- right click on control handle [white square] to access options
- left click on arrows to change direction
- drag control handles

Dashboard

Most features are controlled through the Dashboard at the bottom of the graphics area. This
has icons and popup windows which control the fundamentals of the feature.

Input boxes highlighted in yellow have focus so be careful you put information or references in
the right box.
Solid or Surface

This feature should default to Solid. If the surface icon is highlighted

then check your driving sketch is closed and valid for an extrude

Protrude or Cut

Do you want the created volume to add (Protrude) or subtract

(cut) material from the existing model?

Thin feature

If you are producing a feature which mimics a sheet metal or tubular

part then rather than spend ages in sketcher producing the offset
line for the wall thickness, simply use the Thin option and specify a
wall thickness. Your sketch can then be open or closed.

Depth Control

Use the right click menu via the depth drag handle or the dash board control to change the

depth control. Choosing an appropriate depth control which robustly captures the design

intent

Blind – specified distance

 Symmetrical – specified distance, half each side of the sketch plane

The end surface of the two previous options is parallel to the sketch plane

To Next – continues until next geometry

Through Until – can pass through other geometry to selected reference

The end surface of the previous two options is trimmed by the selected reference – if it’s a
curved surface then the end face will be curved to match

To Selected – as Blind but distance defined by selected reference

The end surface with To Selected will be parallel or trimmed dependent on selected reference

Through All – intersects all features in the model – as the model grows the depths
grows

Develop independently from both sides of the sketch plane

The Dashboard > Options drop down menu also allows you to develop the feature from both

sides of the sketch plane with different depth control options.

Intersecting solid features will simply merge into each other as a single volume, so, if its more

convenient, you can use a datum plane within a solid or extrude through and out the other

side of a solid.

Editing/Modifying Modifying and developing the Model

One of the main strengths of a parametric modeling system is the

ability to develop a model by changing existing features and for that
change to propagate though the whole model.

" With great power power comes great responsibility " - it doesn't
necessarily follow that the model will update successfully, it is your
responsibility to build a robust model which considers the
implication of changes and development, the power to develop a
model can cause references and associativity to fail.

Even with the best planning, features will fall over. A whole list of
features may fail but this is simply a domino effect - if you sort out
the first failure it will often resolve the rest of the list. Make sure
you know how to resolve issues, generally this is as simple as
redefining sketcher references.

Edit Definition
RMB > Edit Definition to re-enter the feature environment and
make changes to the feature.

Edit or Dynamic Edit

The driving dimensions of features can be change without having to

enter the feature environment - Edit Definition. RMB > Edit or
Dynamic Edit will display the features driving dimensions and allow
them to be edited in the graphics area.

If the cursor icon changes when you hover over an element of the
feature it usually means it can be dragged to make modifications.

Ctrl G to regenerate the model and see the effect of your changes.

Dynamic Edit allows you to drag dimensions and see a live update
of the model. This generally applies to any dimension which was
controlled by a drag handle at the feature creation stage.

Regeneration

Any change to the model, however small will generally cause the
model to be Regenerated - rebuilt to consider the implication of
the changes.

Use the Regenerate icon in the top toolbar or Ctrl G to manually

regenerate a model. In assemblies you may have to force a
regeneration if you have made changes to associated parts to see
that change.
Insert Here
Drag the Insert arrow up the model tree or RMB > Insert Here to
insert feature at a specified point in the model tree. Also use this
option to avoid the entire model regenerating with every change.

Suppress

RMB feature in Model Tree > Suppress

This doesn't delete a feature but 'freezes it and takes it out of the
build

RMB > Resume to re-activate the feature

Temporarily suppress heavy features such as patterns or groups of

fillets to reduce regeneration time.

Dynamic edit Xsec

A useful tip which exploits the Dynamic Edit function is the ability to see a live, draggable
cross section of a part (not assembly)

 create a datum plane in such a way that it has a dimension

with a drag handle - say a simple offset plane
 through the View Manager, create an xsec using this plane -
set the xsec as active
 Dynamic Edit the plane and this will dynamically update the
cross section

Managing the model: modifying features and resolving failures

You need to be aware that CAD software is not like most of the software you are used to
working on. Don't expect too many similarities to Word, PhotoShop etc. - this is an industrial
piece of software with a lot of depth and complexity.

Parent/Child Relationships
Just as you cannot exist if your parents did not exist then one feature which is referenced to
another feature cannot be resolved if the reference feature ceases to exist or is fundamentally
altered.

Features have parents and children and you should always consider those relationships when
making modifying your model

Create then Modify

Features are very easily redefined. If something didn’t turn out as you wanted or fails then
you do not have to delete it and start again you simply go back into the feature creation
process and tweak the parameters.

Failed features

If the feature you have created cannot be built or your actions have
effected another feature, i.e. you’ve fundamentally changed or
removed references, then a warning message will give you the
option to undo the changes or continue.

If you continue, the effected feature and any effected child

features in the Model Tree will turn red and be suppressed.
They are not deleted but they are taken out of the build, RMB >
Edit Definition to sort out the failure.

You may need to think very carefully about why a model has failed.
It may be as simple as a failed fillet because you deleted the
reference edge in the sketch driving the extrusion the fillet was built
on. It may be that the changes you made had a 'knock on' effect
through a number of levels of direct child features and children of
children.

File Management: The Working Directory

As Creo works with your model it needs certain configuration and administration files. If it
cannot find these you may have problems with your file later on. In the labs, these files reside
in the Working Directory:

When you create a new file its name and location are set at that point (unlike
common Windows software). The Default folder for files to be saved is again the
Working Directory.

Unfortunately, this is a different location in different labs. Make sure you look at
the address in the Save window:

LDS011: C:\Users\Public\Public Documents\ptc

LDS003: C:\ProgramData\PTC

The address for LDS003 cannot be navigated to through Windows

Explorer, copy it into the Start>Search box to go to that address.

The most efficient working method also dictates that this is also the place from where you
should work on your model files.

 Copy your files [from where they are stored] to this location at the beginning of a
session.
 Work on your files.
 Move them back [to there original address] when you have finished

Which ever piece of software you are working on your should never work from your U: space
or any other storage device – connections can be lost and working speed is always slower.
Getting into good habits early on can save you a lot of heart ache in the future when
the above working regime is even more important.

See Creo Administration for setting up your own installation of Creo

Version files
Each time you save your model, Creo will save a complete new file. If I saved the file
bracket.prt three times I would find bracket.prt.1, bracket.prt.2 and bracket.prt.3 in the
working directory.

This allows you to track changes and revert to previous build states of a model. The highest
number file is the most recent and is the only one you need to keep.

To delete version files of the active model either use the DV icon in the top toolbar, or
File > Delete > Old Versions - take care not to pick All Versions.

Or simply use My Computer to find and delete the unwanted files.

Associativity

First you create your core part files. From these you create assembly files, drawing files and
manufacturing files (which also creates a further .asm file). These subsequent three
files, .asm, .drw and .mfg do not contain the original part files which are used within them.
Each time they are opened or regenerated they will be rebuilt or redrawn according the latest
version of the part file.

For this reason it is essential that you keep all associated files together in one folder and do
not rename them once they have been associated to another file type.

Robust Modelling

In a design environment it is very rare that a model is built and then

never changed, products will go through many iterations at the
development stage and during the lifecycle of the product once it is
manufactured
Don't worry too much about how long it takes to build a model,
more importantly, consider how long it will take to modify it - again
and again and again and..... When you do modify your model, will
everything update nicely or does the whole thing fall over and fail?

Don't be afraid to test your model, change dimensions, change references and
see what happens - make sure you save it first!

Modelling Strategy

When visualising part of a product we tend to see it as a complete

form. Prototyping will tend to be a subtractive process where we
start with a lump of material and remove material to create the
desired shape. 3D CAD on the other hand

Efficient Modelling

Revolve

The sketched section curve rotates around an axis which must be on the same plane [planar
surface or datum plane] as the sketch. The axis could be:

 an existing straight edge

 an axis

 or, the simplest method, a centreline drawn within the sketch

The sketch must, logical, be on only one side of the axis.

Blend - Swept Blend

Key Terms:

Sections
Vertices
Blend vertex
Start point
Trajectory

DO NOT use Insert > Blend to produce a blend. This is a

legacy feature which uses the Menu Manager interface.

The Swept Blend uses the Dashboard interface and is

therefore quicker and simpler to set up and modify.

The blend function in Creo is commonly known as a loft [originating from boat building] in
generic CAD terms. In its simplest form we would have multiple parallel 2D sections which
are spaced apart from each other. The CAD system creates a volume (solid, cut or surface)
by filling in the gaps between these cross sections.
There are two main issues which need addressing when creating a blend feature; number of
vertices in each section and alignment of the start points.

Number of Vertices
In the example below, a circle has been blended to a hexagon. The lines which join the two
sections and represent the volume of material to be created are joined from vertices [points
where curves meet] on one section to vertices on the next.

But if, as in the above left example, there are an different number of vertex's in the two
sections [a circle has no vertex's!] then the systems needs to be told where to connect the
points to. In this case the circle has been split into six arcs.
We could have split the circle into less segments and created a blend vertex - essentially a
point on top of a point which would allow us to connect two points from the hexagon to one
point on the segmented circle. This would give a very different form.

Start Points
In each of the sections one of the vertices is designated as the start point. These are the
first points to be joined between the sections, the system then moves logically around the
sections joining each point in turn.

Where your start points are placed decides on the final form. This can be seen in the two
images above where the start point has been moved in the second model giving a very
different form.

Decisions concerning numbers of vertex's and start point positions is very much based on
your Design Intent.

Functionality

Common Considerations:

 As with any blend, each cross section must have the same number of vertices
(points), or in other words, be made up of the same number of lines. This defines
how one section is connected to another.
  Try and plan the feature so that the section are not swept around the inside of any
curves in the trajectory - problems can occur if the section has to be ‘compressed’
inside a tight curve.
 The cross sections and the trajectory can be sketched or selected from existing
edges or reference geometry - selecting existing geometry is more robust.

External Sketches

Creating your trajectory and sections as separate features is a more efficient strategy as
you will not lose your construction geometry if the features is deleted

Pick the Swept Blend icon from the right toolbar.

Solid or surface? This feature defaults to surface, so pick solid if that is what you want

Watch a video HERE

Trajectory

The first element you need to select is the Trajectory

Although to produce a simple Blend the Swept Blend needs a trajectory, it could be as
simple as a straight line or an existing edge.

The blend will only be created as long as the sections are within the extents of the trajectory -
make sure the trajectory starts before the first and extends past the last section
Using the right click menu for options is usually quicker.

Select a sketch or edge[s] to define the trajectory.

Sections

Through the right click menu or under the Sections option change to Selected Sections

Pick your first sketch, then pick Insert [right click menu or Sections option again] to add to
the list and then pick the next sketch along the trajectory.

Continue to pick Insert and select the relevant sketch for all your sections.

If your section is made up of multiple edge elements then you will have to create a 'chain' of
edges.
DO NOT use CRTL to pick multiple solid edges as this will select multiple sections.

To create a chain of edges:

 Select the first edge

 Press and hold SHIFT
 Pick the first selected edge again - this changes the selection method to chain
 Still holding SHIFT, select the other edges which make up the chain

If the previewed solid is twisted because the start points are not aligned, simply drag the start
point marker to the appropriate vertex.
Blend Vertex

You may have a situation where you have an unequal number of vertices but its not
appropriate to split one of the curves because you want multiple points in one section to blend
to a single point in the next - imagine a square blending to a triangle. In this case you need to
add a Blend Vertex - basically a point on a point to increase the vertex count.

Continue the process as before. When you come to the section which needs a blend vertex
use the Add Blend Vertex button in the Sections menu. The extra point will show as a
white square, drag this to the appropriate vertex.

You CANNOT have a blend vertex on the Start Point, if they coincide, move the start point
on your sections
Tangent end conditions

If the feature is joined to a suitable geometry you can use the end condition markers to set
tangency. In the below example some simple control surfaces were created prior to the
swept blend feature to enable setting tangency.

Constant Section Sweep

Use the Constant Section option in the Variable Section Sweep [VSS] in the right hand

toolbar

The main issue when creating simple sweeps is the placement of the 2D sketch – the section
– relative to the path it is to follow – the trajectory.
In the above example two identical circles have been swept along the same trajectory – the
centre of the circle remains the exact same distance from the trajectory at every point and the
cross section remains normal [at 90 degrees to] the trajectory at every point.

With the same trajectory and section, two very different forms have been created.

The issue with the circle on the inside of the trajectory is that it is self intersecting – the
volume of material is overlapping itself.

Method

Watch a video HERE

VSS > right click > Constant section

Select your Trajectory

Either select a predefined sketch or select edges. Only select a single trajectory.

If your trajectory is a made up of a number of curves or edges - a chain - do not use crtl pick
to collect the curves/edges:

Selection method:

- select the initial 'anchor' curve/edge

- hold the SHIFT key

- hover over the segment you you are working on and press shift to see the pop-up hint
'one-by-one'

- press hold the shift key.

 - select the segments you need for the chain. Remember you can right click to toggle
through the selectable segments. Also look for a Tangent Chain to highlighted.

Section

Right click menu > sketch

No visible datum plane is created, the sketch plane is simply represented by the yellow xy
vector reference lines. By default the plane is created normal to the end of the trajectory.
Tumble your view to make sure you can visualise the sketchplane position and orientation.

You cannot select an existing section - this will have to be sketched within the feature. This
is because a sketch plane is set up relative to the selected trajectory.

You can use an existing section by using the copy edges function in sketcher. Remember to
consider whether the sections sketchplane is normal to the end of the trajectory.

Swept blend utilising reference geometry

The Swept Blend creates a feature which is defined by two or more cross sections
positioned along a trajectory - the resulting form is influenced by the sections and the
trajectory.

In the example below, the edge of the model is used as the trajectory and three different
sections are placed along the trajectory.
In the above example the dimensions of the 'L' shaped lip change as it sweeps around the top
edge of the base feature - these dimensions are controlled by the 3 sections positioned
around the edge.

Common Considerations:

 As with a blend, each cross section must have the same number of vertices (points),
or in other words, be made up of the same number of lines. This defines how one
section is connected to another.
 Try and plan the feature so that the section are not swept around the inside of any
curves in the trajectory - problems can occur if the section has to be ‘compressed’
inside a tight curve.
 The cross sections and the trajectory can be sketched or selected from existing
edges or reference geometry.

Pick the Swept Blend icon from the right toolbar. The system defaults

External Sketches

Creating your trajectory and sections as separate features is a more efficient strategy as you
will not lose your construction geometry if the features is deleted

Trajectory

Select a sketch or solid edges to define the trajectory. If your trajectory is made up of multiple
edge elements then you will have to create a 'chain' of edges. DO NOT use CRTL to pick
multiple edges as this will select multiple trajectories.

To create a chain of edges:

 Select the first edge

 Press and hold SHIFT
 Pick the first selected edge again - this changes the selection method to chain
 Still holding SHIFT, select the other edges which make up the chain

Sections
Under the section options change to Selected Sections. Pick your first sketch, then pick
Insert to add to the list and then pick the next sketch along the trajectory. Continue to pick
Insert and select the relevant sketch for all your sections.

If the previewed solid is twisted because the start points are not aligned, simply drag the start
point marker to the appropriate vertex.

Tangent end conditions

If the feature is joined to a suitable geometry you can use the end condition markers to set
tangency. In the below example some simple control surfaces were created prior to the
sweptblend feature to enable setting tangency.
Engineering Features

Round or Fillet

Chamfer

Hole

Shell

These are features which modify existing solid material.

 Round - Fillet

Removes material to create a radius on a chain of edges. This could be a single radius along
the length of the chain or the radius could vary in size along the chain. The system
automatically creates a chain whilst there is a tangent relationship between edge endpoints.
In the example below only one edge was selected but a chain is formed of the three
tangential edges.

Organise similar or consecutive fillets under one feature where possible rather
than having a long list of fillet features in your model tree - a neat concise model
tree gives a more easily managed model.

Hold the Ctrl key to 'collect' the edges you want to fillet. Use the right click menus on the
drag handles [as above] for different options. Make sure you experiment with the dashboard
options.
Rounds can sometimes fail – particularly at points where multiple edges join without
tangency. Try and visualise what you are asking the system to do.

Auto Round Tool

Insert > Auto Round

This tool will allow you fillet all [possible] edges - concave, convex or both. Once all are
selected you can Exclude edges.

Caution - fillets add a lot to the regeneration time and file size. Sometimes, it is worth
suppressing fillets whilst developing the rest of the model and then resuming them when
finished.

Chamfer

This is similar to a round except that it creates a flat rather than a radius. By default the flat is
created an equal distance from the edge into the two adjacent surfaces. This can be changed
to be unequal using distances or a distance and angle.

As with fillets, organise similar or consecutive chamfers under one feature where
possible rather than having a long list of fillet features in your model tree.

Hole
As the name suggests, this function creates a hole. At its simplest this can be a parallel, flat
bottomed hole. Or it could be a hole with a custom profile driven by a sketch. Or it could be a
‘standard’ hole whose profile is specified by a standards agency such as ISO or ANSI.

As with any other feature, the hole must be robustly referenced. It must be placed on a
planer surface or datum plane and its position on that entity must be fully explained from
appropriate references.

Placement surface - the surface you are going to 'drill' the hole into can be either planar,
cylindrical or conical. The hole axis will be normal to this surface.

If the surface you want to 'drill' into is not planar, cylindrical or conical [ie. a complex 3D
surface] or if the hole needs to be at an angle to the placement surface then you will need to
create a datum plane in an appropriate orientation to use as the placement surface. For a
complex 3D surface you could also use a point on the surface but the hole would then always
be normal to the surface at the point.

Primary reference - this is not always the placement surface. This is the most significant
reference in placing the hole. It could be a planar, cylindrical or conical surface, or it could be
an axis or a point. Depending on what you choose will dictate what other references are
required.

Offset References - defining the position of the axis on the placement surface - access via
right click menu or Placement drop down. Different types of positioning references will be
required according to what type of placement reference you have chosen. Planar surfaces
and datum planes are common picks for this references.

Linear - dimension from X and Y references - these must be perpendicular to the primary
reference. Surface/plane as placement reference

Coaxial - the hole axis is aligned with an existing axis. Crtl pick axis and surface/plane in
placement box.

Radial/Diameter - the hole axis is placed at a radius/diameter from a reference axis. It also
needs an angular dimension 'around' the axis from a chosen plane which is parallel to the
hole axis. Surface/plane as placement reference, change Type to Radial/Diameter, axis and
perpendicular angle surface/plane as Offset references.

Combinations:

Planar placement reference - positional references could be linear, coaxial, or

radial/diameter.

Cylindrical placement reference - this will require a linear reference to place the hole along
the cylinder and a plane parallel to the cylinder axis to give an angular reference.

Conical - this requires the same references as a cylindrically placed hole. The linear
reference will translate the the distance along the angular surface.

Point - if a point is chosen as the primary reference then the hole axis will be normal to the
surface the point resides on.

Shell

This feature removes the internal volume from a solid leaving a specified wall thickness.
Selected surfaces of the solid can be removed to create an opening to the internal void or it
can be left as a closed shell.

The shell feature generates offset surfaces for all solid surfaces which exist at
that point in the build process, carefully plan the position of the shell - geometry
which does not need to be shelled must exist after the shell process. There
should generally only be one shell feature in a model otherwise you will be
shelling the shell!

Ctrl select the surfaces you wish to remove to 'open' the volume, you do not have to select
any surfaces, you may want a closed shell which may be opened up later by other features.

Shells can be a problematic feature if the solid has complex geometry. Sometimes you will
have to think of a work around to achieve your design intent.
Additional useful Engineering Feature:

Draft feature

The draft feature is commonly understood with respect to mould tools. It will add or subtract
material to a group of edges to the set draft angle.

4 elements:

1. Draft surfaces - those surfaces to which material will be added or subtracted

2. Draft hinges - the edges about which the surfaces will rotate - these do not have to be
adjacent to the draft surfaces

3. Pull direction - in the above scenario, either the chosen edge or the bottom surface
indicates the zero degrees vector - vertical

4. Draft angle
Edit Feature: all in right toolbar

Key terms:
Mirror
Pattern
Copy
Paste
Dependency

Dependency

Often, when you create a copy of an entity there will be an option to make the copy
dependent or independent of the original. Any changes in the original entity will or will not
be reflected in the copied instances.

Mirror

To create a mirrored copy of a single feature, number of features or group simply make your
selection in the model tree, select the mirror tool and then select the plane about which the
features are to be mirrored.

Model Symmetry

You can also mirror the entire model tree by selecting the model name at the top of the model
tree and then selecting the mirror function. This more robust than mirroring a selection of
features as it mirrors all the elements needed to create the mirror geometry.

Dependent or Independent

You will notice that two different icons (as above) are used in the
model tree when you mirror features. Dashboard > Options >
Copy as Dependent will be ticked by default if it is possible to
create an associative mirrored feature – one which will update to
follow the original. If you cannot create a Dependent copy then try
grouping the feature with its construction geometry and mirroring
the group.
 Pattern

To create multiple instances [copies] of a feature or features in a regular pattern [or to fill a
prescribed area] you can select the items and then use the pattern tool [or right click >
pattern].

Patterns can be linear - line or grid, radial - referenced to an axis, or follow a curve.

All patterns need references to define their direction and characteristics.

The dashboard controls firstly define the type of pattern, this will then dictate which direction
reference boxes are displayed. The number of copies in each direction is also displayed.

Remember to use your right click menus as well

Simple patterns - Direction, Axis, Fill, Curve

These pattern types are the simplest to set up but do not give any control over the geometry
in the individual copies.

Direction - choose a plane/surface to signify a direction

Axis - choose an axis to signify the centre of rotation

Fill - choose a sketch as a boundary to fill

Curve - choose a sketch to follow

Axis pattern, equal spacing

Patterns with geometry control - Dimension pattern

A Dimension pattern will allow you to control the geometry and position for individual copies.
This patterns form is dictated by the direction references you choose - linear, radial or curve.

Driving dimensions

As with any other features, a pattern requires references. The important concept to
understand with patterns is that you choose parameters [dimensions] which place the original
feature to describe the direction or nature of the pattern.

The chosen dimension also indicates the positive direction. If you want the pattern to
increment in the opposite direction you need to input a negative figure.

For a linear pattern [as above] dimensions in X and Y which place the original feature are
selected to indicate the two pattern directions. These references are placed in the two
Dimension boxes - Direction 1 and Direction 2.

Radial pattern

The driving dimension for a radial pattern [below] is the angular dimension placing the
original feature.
The dimensioning scheme for a radial Dimension pattern must be carefully considered. The
default linear placement of the sketch in the below left image will conflict with the radial
pattern. The modified dimensioning scheme will produce a successful pattern.

Incrementally changing instances

You can also change the parameters of a feature as it is copied – eg. each instance decrease
progressively in height through the pattern.

In the above example an extrusion has been patterned around the axis of the base cylinder.
This pattern has then been altered so that as each instance of the original extrusion is
created, the height dimension, the diameter dimension and the distance from the axis
dimension are adjusted.
The parameter you wish to change is included in the appropriate direction box and the
incremental adjustment input. In the above example the height dimension, diameter and the
distance from the axis dimensions are collected in the Direction 1 box after the initial angular
driving dimension.

Copying features

You can use the Copy, Paste, and Paste Special commands to duplicate and place features,
geometry, curves, and edge chains. Using this functionality, you can copy and paste features
within the same model or between two different models.

By preselecting edges you can create a copy as a datum curve either as an exact copy or
an approximate copy – this will approximate a chain of tangent curves as a single continuous
curvature spline curve.

Two methods for Pasting solid features:

 When you use Edit > Paste, the system opens the feature creation tool, so you can
redefine the copied feature.
 When you use Edit > Paste Special, the system allows you to replace the original
references with the new ones.

Reference geometry
These features do not form part of the model but are created in order to establish a reference
for model features where no suitable reference exists - remember, everything has to be ‘fixed’
in our 3D space.

Degrees of Freedom (DoF) – the freedom to move in a direction which has not been
constrained – fixed to another entity. Can the entity be moved in any direction or rotated?

The reference geometry you create also has to referenced in space such that it has no DoF.
You will not be allowed to complete the feature until all the DoF have been resolved – until it
has been fully constrained. How many references or constraints are needed to place your
new reference feature is dependent on what sort of geometry it is and what you are
constraining it to.

To 'collect' references

Whenever you are presented with a references window you will need to hold the Ctrl key if
you need to 'collect' multiple references - standard Windows functionality.

Normalcy - the term normal is generally used instead of perpendicular or orthogonal to

describe a line or axis being at 90° [in all directions] to a plane or surface.

Planes:
parallel offset from another plane/surface

normal to a plane/surface

through an axis/line/edge/point

angular offset from another plane [must be combined with through axis/line/edge]

Points:

DO NOT put datum point on curve ends or surface edge ends - these are vertexes and are

already seen as points which can be connected to.

Constrained to other references:

On a surface/plane and referenced to other entities, ie. two other surfaces

On an edge/line relative to the end of the edge, line

On an axis relative to another reference

Offset from a csys in x,y and z

Sketched on a surface/plane

If you are creating multiple points then include them all in one feature if possible – this can

result in a significantly shorter and tidier model tree.

Axis:

Through a point/vertex/curve/edge

Normal to a surface [doesn’t have to be planar] or plane

Curves:

Sketched on a surface/plane

Thru Points - a curve can be constructed to pass through any number of points -

reference points, vertex's, curve endpoints - in space

Projected onto a surface

Helical Sweep

Springs and screw threads are the classic examples of using a Helical Sweep, but think
about how you might produce a knurl pattern using this functionality. Think of this feature as
a standard sweep along a helix.

Unfortunately this function is still under the 'Menu Manager' interface.

Insert > Helical Sweep > Protrusion or Cut

The feature properties window opens up and starts with the features attributes.......

Attributes

Constant or Variable pitch?

Definition: the distance travelled along the axis for each 360 degree revolution of the helix.
In this section we shall just deal with a constant pitch, go to the end of the section for
guidance on setting up a variable pitch

Section Orientation?

This defines whether the section sketch plane remains vertical - parallel to or through the axis
[default] - or if it is normal to the trajectory of the sweep.

The effect of this choice can be best seen in a sweep with a 'fast' helix - a pitch greater than
the profile length. In the image below you can see the sweep section is distorted if the option
Through Axis is used [feature on left] - the sketch plane is at an acute angle to the trajectory.

The feature in the right of the image looks more like a standard sweep - the sketch plane is
always Normal to the trajectory.

Right or Left Handed?

Simply the direction of the helix. A standard screw thread is right handed.

Done

Consider the sweep from the side view, we first need the sketch plane for the axis and outer
profile.

Direction [view direction onto sketch plane] > Okay or Flip

Sketch plane orientation - pick direction, then pick a perpendicular plane to face in that
direction.

Now you are ready to sketch the cross section of the form.

Swp Profile

Create a centreline as the sweep axis.

Create a line to show the outer profile of the sweep - this does not have to be vertical or even
a straight line [draw this to the left of the axis to avoid confusion in the section sketch]

Complete the Sketch

Pitch

This is the distance the helical 'spiral' moves along the axis for each 360 degree turn. Input a
figure in the prompt in the text area of the screen and hit the tick.

You will then enter a 2nd sketch environment to create the cross section of the sweep

Section

Make sure you identify which reference is the axis and which is the outer profile as its an easy
mistake to draw the section up against the axis!

Complete the sketch

Variable pitch

Select Variable rather than Constant pitch [second feature in top image above]

The Profile can still be any shape.

A single line will allow a start and end pitch with a smooth transition from one to the other over
the length of the sweep.

If you want the pitch to be different values at various points along the profile then you need to
break the profile into sections at the points you want the pitch to vary.

You will be prompted for the start and end pitch.

A graph will then appear which shows the pitch along the profile. Pick the break point on the
profile sketch to add them to the graph and define a pitch at that point.

If you want to change the values, use the Change Value option in the Pitch > Define Graph
menu.

Level 2 Modelling
The main emphasis at this level will be on more complex modelling strategies and planning.
Your models should be more robust and flexible - if you make a change to feature no.5 of 100
how many failed features are you going to have to deal with?

Your design intent should be fully captured in the chosen references and dimensioning
schemes. We will also look to improve and consolidate skills gained in Level 1

We shall also be introducing Surface Modelling techniques to

create forms with complex curved surfaces with cannot be achieved
through standard modelling functionality.

Modelling Functionality to date

Base features:
 Extrude

Revolve

Sweep – by default use the Variable Section Sweep function

Blends [Loft]

Swept Blend

Boundary Blend - surface modelling

Engineering Features: all in right toolbar

Round [fillet]

Chamfer

Hole

Shell

Edit Feature: all in right toolbar

Mirror

Pattern

Reference geometry
These features do not form part of the model but are created in order to establish a reference
for model features where no suitable reference exists - remember, everything has to be ‘fixed’
in our 3D space.

Degrees of Freedom (DoF) – the freedom to move in a direction which has not been
constrained – fixed to another entity. Can the entity be moved in any direction or rotated?

The reference geometry you create also has to referenced in space such that it has no DoF.
You will not be allowed to complete the feature until all the DoF have been resolved – until it
has been fully constrained. How many references or constraints are needed to place your
new reference feature is dependent on what sort of geometry it is and what you are
constraining it to.

Planes:

parallel offset from another plane/surface

normal to a plane/surface

through an axis/line/edge/point

angular offset from another plane [must be combined with through axis/line/edge]

Points:

Constrained to other references:

On a surface/plane and referenced to other entities, ie. two other surfaces

On an edge/line relative to the end of the edge, line

On an axis relative to another reference

Offset from a csys in x,y and z

 Sketched on a surface/plane

If you are creating multiple points then include them all in one feature if possible – this can
result in a significantly shorter and tidier model tree.

Axis:

Through a point/vertex

Normal to a surface [doesn’t have to be planar] or plane

Curves:

Sketched on a surface/plane

Between two or more points - consider end conditions – tangent, normal etc.

Attribute > Quilt/srf - once a curve between points has been created it placement can be
changed from free [the shortest, smoothest path between the points] to lying on a surface.
The points will need to be on the surface before this can be applied.

Tangency end conditions - if the curve is referenced through its start point to another entity
[ie. it starts from the vertex of an edge or from a point on a surface] a normal, tangential or
curvature continuous relation can be created.
Sweep curve [Coach example here]. A curve between multiple points can be given the
condition ‘single radius’. The points are then joined with straight lines and then a fillet
[round] is created an the junctions – ie. consider the sweep path for a bent tubular steel chair

Intersect – create curve at the intersection of two preselected entities – Two sketched
curves, two surfaces, a plane and a surface.
Project – an existing curve or a sketch can be projected normal to a selected plane onto a
surface

Wrap – whereas a projected curve will be distorted if it is created on a non planar surface, a
wrapped curve will not be - it will form across a surface such that all the curve lengths are
unchanged.

Note: you cannot wrap a curve onto a surface which is curved in two directions - only
cylinders.

To Wrap onto complex surfaces

If you need to apply some curves to a surface with curvature in two

directions whilst minimising distortion you could:

 create a cylinder which approximates in orientation and

diameter to the target surface
 create your sketch and Wrap onto this cylinder
 create a sketch from the wrapped curves - Sketch > Copy
Edge tool
 use the appropriately distorted sketch in a Project or Offset
surface process onto the target surface
If your target surface is tending to the spherical you will still get
distortion in one direction, make sure you align the cylinder with the
direction of least distortion.

Offset Curves

To create clearance between assembled parts which may be the

result of a Top Down Modelling (see Assemblies) approach, you
may need to offset edges or curves.

Note: you can Offset curves or surface edges, you cannot offset
solid edges. Copy the surface edge first (select, Ctrl C, Ctrl V) and
offset the copy

The Offset tool is selection driven - select the geometry to enable

the tool

To select solid edge: select solid, select surface, select edge

To select surface edge: select surface, select edge.

Edit > Offset

Variable Section Sweep

A standard swept feature [created under the same function] has a single trajectory and a
constant [unchanging] cross section. The Variable Section Sweep (VSS) has an initial cross
section which is referenced to multiple trajectories which influence [distort] the section as it
travels along those trajectories.

Therefore, you cannot use an existing sketch or edges for the VSS section as it would then be
referenced to that section and not be able to ‘distort’. As you cannot reference to a start or
end section this would not generally be used as a fill between existing end sections.

Key points:

 Trajectories must be tangent chains

 Dimensions of the section vary but not the fundamental geometric elements
 A high level of control is maintained over the length of the resultant form
 The dimensioning scheme must be carefully considered – which dimensions are fixed
and which are allowed to vary
 Reference to existing geometry with care
  Sketchplane placement is greatly effected by chosen trajectories and which is the
origin
 There is a need to experiment with the combination of setting in terms of origin
selection and section alignment

Because it is a more complex feature a thorough initial analysis of the planned form and the
trajectories and section is needed. Then an understanding of how the feature is developed
using this structure - this feature generally needs some fine tuning before it is successful.

Sketchplane

The sketch plane has to intersect all trajectories. The resultant solid cannot extent beyond
the selected trajectories and therefore the trajectories need to be carefully considered in
terms of the section orientation control.

Section normal to
origin trajectory -
top curve

Section normal to
origin trajectory -
bottom curve
 Section parallel to
end plane -
'constant normal
direction'

Section behaviour

One the key concepts to understand with the VSS is how you influence the orientation of the
section as it progresses along the trajectories. Experimenting with the order in which you
select the trajectories and which section control option your choose is the key to success with
this feature

The first trajectory you choose is the origin trajectory and by default the section remains
normal [Normal to Trajectory] to this curve as the feature develops.
Related subject: Trajpar - go to the Relations section

Layers & visibility

Layers – features organisation, ruled layers, setting rules

View manager - sections, custom view states

Advanced Rounds

Intent edges

When selecting edge references for a round feature, either toggle

(momentary RMB) or RMB > Pick from list and you will find Intent
Edges – edges which define the design intent. This edge chain or
collection of edges is identified by the surrounding features and not
by the edge identity.

In the example above, three Sets were created containing a single

Intent Edge reference in each – Intent Edge in Set 1 includes the
four vertical edges, Set 2 is the top loop and Set 3 is the bottom
loop.

Above left is the initial result. If the driving sketch is altered to

produce the section as above right, then the design intent captured
in the Intent Edge references is recognised and the round edge
chains are redefined accordingly. If you had chosen individual
edges then the rounds would have failed when the section was
changed.

Round sets

If you have multiple edges or chains which have a common size fillet
then manage those edges under one feature. Hold the Ctrl key to
'collect' the edges you want to fillet. Use the RMB menus on the
drag handles (as above) for different options. Make sure you
experiment with the dashboard options.

If you select a subsequent edge without holding Ctrl then a new Set
of edges will be created. Each edge Set has unique parameters.
Manage Sets through Dashboard>Sets

Transitions/stops

At some point, fillet edges will meet each other in the model, the
fillet surfaces will have to be ‘blended’ together – this is the round
transition. Pick on the Transition icon in the dashboard, select a
highlighted transition on the model and, depending on the
geometry, you may be given different options for the shape of the
transition.

Full round
If you create a fillet on two parallel surface edges to such a size that
it consumes the parent surface between these two edges it is
referred to as a Full Round. Select the two parallel edges > pick the
Full Round option.

Relations - Mathematically Controlling the Model

Creo Help > Fundamentals > Relations and Parameters or PTC_U > Advanced Modelling >
Relations and Parameters

ProE models are driven by parameters, all model parameters have an identity;

Right click > Edit a feature in the model tree

This will show all the feature parameters in the graphics area

Info > Switch Dimensions will show you the parameters identities

Select a parameter in the graphics area > RMB > Properties > Dimension Text > Name
allows you to change the name of the parameters giving the parameter a more logical name
to use in relations.

These identities can be used in a mathematical equation to control the model. This can
control can be at the Sketch, Part or Assembly level. This is a powerful tool for robustly
capturing Design Intent and controlling the models behaviour.

Depending on your maths skills, you can take this control as far as you want using traditional
operators and functions in equality or comparison controls, ie. d34=d6*7, d5 =
d2*(SQRT(d7/3.0+d4)) or IF d1 > d2, length = 14.5, ELSE , length = 7.0, ENDIF

User Defined Parameters

You can also create a list of unique parameters to use in relations which might defines say a
general shell thickness, common hole size or clearance value. The CLEARANCE parameter
below could be used to set all clearances on an injection moulded assembly, the one
parameter simply has to be changed to change the whole assembly.
Creating Relations

In the Sketch, Part Or Assembly: Tools > Relations to enter the Relations dialogue box

If your in sketcher, the parameters will change to IDs

If your in part or assembly mode, pick the features [model tree or screen] to show their IDs

Pick those IDs on screen [or simply type them] to include in the equation

Driving Dimensions with Parameters

Create Relations as above use the Parameter name in the relation statement,
eg. D6=clearance1 The Parameters can viewed and changed at the bottom of
the Relations window. The model will have to be regenerated (CtrlG) to effect
any changes.

Trajpar in VSS
Trajpar is a unique parameter which is used in the Variable Section Sweep function and is
related to the Origin Trajectory length. This parameter varies from 0 to 1 as the sweep
develops along the the trajectory.

O at the beginning of the trajectory, 1 at the end of the trajectory, therefore 0.5 half way along
etc.

This parameter can therefore be used to control the sweep section within a relation.

Example: 'Traditional' telephone cable

You cannot produce this form with a helical sweep as it would need to be a linear trajectory,
so this method uses a VSS and Trajpar

Create a curve which represents the path of the cable - Curve thru' points, intersect curve or
Style curve

Start a VSS and choose this curve as the trajectory - leave as Surface not Solid. Enter
sketcher.
Construct a simple short line (sd6 above) attached to the end of the trajectory as above.
Notice the dimensioning scheme - line length and angle

The angle [sd5] will be controlled by the relation: [angle] = (360*trajpar)*30 - ignore the *30 for
the moment.

- Trajpar = 0 at the traj start

- Trajpar = 1 at the traj end

- at the traj start the angle = 0 deg.

- half way along, trajpar = 0.5, angle = 180 deg.

- at the traj end the angle = 360 deg.

The *30 means this happens 30 times over the length of the trajectory - 30 coils. Change the
30 for more or less coils.

The outer edge of the spiralling surface is then simply used as the trajectory for a constant
section sweep.
Draft feature

The draft feature is commonly understood with respect to mould tools. It will add or subtract
material to a group of edges to the set draft angle.

4 elements:

1. Draft surfaces - those surfaces to which material will be added or subtracted

2. Draft hinges - the edges about which the surfaces will rotate - these do not have to be
adjacent to the draft surfaces

3. Pull direction - in the above scenario, either the chosen edge or the bottom surface
indicates the zero degrees vector - vertical

4. Draft angle

Silhouette Trim

Useful for finding your split line on complex surfaces eg. creating a mould tool;

Select your solid surfaces - select one surface > RMB menu > Solid Surfaces

Copy and Paste to create Surf Copy feature

select the Copy feature - Edit > Trim

select a plane/planar surf parallel to your split

choose the Silhouette option in the dashboard

choose which side to keep

Hide instances - pick black preview dot whilst creating the pattern to hide that instance

Reference pattern - if you reference a new feature to a pattern instance, say filleting the
edge of a patterned hole, and then pattern the new feature, the system will recognise the
relationship and create the new pattern as a Reference pattern following the underlying
parent pattern instances

Unpattern - if you pattern a group of features, the pattern can be 'exploded' so that the
instances are independent. RMB the pattern in the Model Tree.

Pattern regeneration time - patterns can take a long time to regenerate, these methods can
save you time;

 Suppress pattern whilst working on other things

 Can you consolidate the patterned form as a neutral model - good for assembly
patterns.
 Create a surface copy of the feature. Solidify inside the volume. Group the surface
and solidify feature together and pattern the group

Creating Geometry from a 2D Graphics Source

At some point you may need to replicate some existing graphics such as a corporate
logo, here are a number of methods.

Vector based software

In the graphics industry logos are generally created in vector based packages such as
Adobe Illustrator or Corel Draw. The linework is maths based and, unlike a bitmap, is
scalable without losing any definition. [Definition: en.wikipedia.org/wiki/Vector_graphics ]

Neutral, industry standard vector files such as .dxf or .dwg can be exported from these
packages and opened directly into ProEngineer. This geometry can then be the basis of
a reference curve.
Illustrator

Bitmap preparation - your starting point is likely to be a .jpg or .gif bitmap file. You may
need to do some work on your image in Photoshop to give a better contrast to the
required edges - look at simple Image > Adjustments > Brightness/Contrast or have a
play with Image > Adjustments > Levels.

In Illustrator you can File > Place a pixel based image into an empty document

Select the image > Object > Live Trace > Make to find boundaries of high contrast.
Expand in the top options to create paths/vectors - at all stages you will have to
experiment with the various options.

** Save as CS version, not a CS2 and untick all Options **

Lots of tutorials for Live Trace out there - eg. LINK

Whilst in Sketcher:

Whilst in Sketcher in ProE you can use the Sketch > Data from File command to import
the .ai file.

Caution: The more accurately the paths follows the selection the more control points are
created in the resulting spline curve.
Firstly this can mean it takes a long time to process the data in sketcher. And secondly a
spline curve should always contain the minimum number of control points. So try and
minimise the number of control points by having the tolerance figure as high as possible.

To reduce the number of points in the spline curve; whilst in sketcher, select the spline
and pick the modify icon. Control points can then be deleted. Check out thee curve
analysis tool at this point as well to get your spline nice and smooth.

Establish tangency, reduce the number of points and smooth the curve.
Bitmaps directly into ProEngineer

When you change the colour of an entity in ProE you create a render swatch which is
applied to the part or surface. There is the option when creating the swatch to apply a
bitmap image.

If you create a closely cropped bitmap image of the graphic this can be used in the colour
swatch which can then be applied to a surface in your part file. The easiest method to get
the image to the correct size is to create a Fill surface [Edit > Fill] from a rectangular
sketch of the correct size. A reference curve can then be created by tracing the image.

For a simpler method look at Level 3 > Reverse Engineering > ISDX Trace Sketch

Model Analysis
Useful Tools

Global Interference will show any overlapping volumes in an assembly

Analysis > Model > Global Interference

Mass Properties will give you the volume/weight of a component or assembly.

The figure for volume is likely to be shown as an exponential figure in the modelling units.

In the example above VOLUME 8.5010447e+03 MM^3 , move the decimal place plus 3
places to give 8501.0447 MM^3. Remember to convert this figure if you need different
units:

1000mm^3 = 1cm^3 8501.0447mm^3 = 8.5cm^3 [approx]

Accuracy

When discussing the manufacture of a part DO NOT say it has to "very accurate" or
"exact", there is no such dimension as 10mm, a part is made to 10mm plus or minus a
certain Tolerance that is its Accuracy.

As well as considering simple dimensional tolerance of a feature, say plus or minus

0.01mm on a length or diameter, we also have to consider the Geometric Tolerance of a
feature - how flat or how round something is, what the envelope of deviation is - Wiki
discussion
Making something to a high tolerance is not necessarily a good thing - high tolerance
costs money and artifacts should be made to an appropriate tolerance - we would not
build a shed to the same tolerance as we would manufacture an analogue wrist watch!

The main reasons for being aware of accuracy in the virtual CAD model are regeneration
times and interaction between parts with differing accuracies. The real world impact of
accuracy setting would only come into play if you worked with, for example. very large
parts or very high accuracy (aerospace) parts.

ProE provides two methods to define accuracy: relative and absolute - the default is
relative accuracy.

Relative Accuracy - the part accuracy is Relative to the greatest dimension of the part.
The default setting is 0.001, therefore the accuracy of our 2m by 1m shed would be 2mm
and a 3mm part in our watch would be .003mm

But what if you have a 10mm cube part which has a long thin tube protruding from the
side? If the tube was 1m long your Relative accuracy would be 1mm - not good for the
10mm lump on the end. This may be a situation where you switch to;

Absolute Accuracy - an absolute figure which all features are calculated to. In the
above scenario we may switch to an Absolute accuracy of .01mm

Another factor to consider if your thinking of making large components to a high accuracy
is Thermal Expansion - a 1m length of aluminium will increase its length by 0.23mm if its
temperature is raised 10 degrees. Environmental conditions need to be conditions with
reference to tolerancing scheme.
Skeleton based surfacing : Fundamentals

Definitions

Surface - is an area boundered by edges which is non solid feature with no thickness
Surface Patch - an individual boundered area with no other edges intersecting it
Surface Quilt - a number of patches joined together
Curvature - with respect to a spline curve or surface with a constantly changing radius. At
any point on the curve/surface its curvature is 1 divided by the radius at that point.
Therefore, a nearly flat area of a surface/curve [very large radius] has a very small
curvature.

Surface Display

The one-sided outer edges of a surface feature are displayed in cerise [pink].
The two-sided inner edges are displayed in magenta [purple].
Therefore a quilt will be displayed as a number of magenta lines inside a cerise boundary.

Surface Continuities

Make sure you know what a spline curve is [HERE] and what curvature is [HERE]

Continuity between surface patches is important for both aesthetic and functional
reasons. Poor continuity can show creases and show each individual patch's boundaries.
Continuity between curves and surfaces can be expressed as geometric (G0, G1, G2)
continuity.

G0 Continuity: Positional continuity. Two curves that share an endpoint, two surfaces that
share a boundary are G0 continuous.
G1 Continuity: Tangential continuity. Two curves that share an endpoint, two surfaces
that share a boundary are G1 continuous when the normals at the join/boundary are
exactly aligned in direction - at that point they are travelling in the same direction.

G2 Continuity: Curvature continuity. Two curves that share an endpoint, two surfaces that
share a boundary are G2 continuous when they have the same curvature values where
they meet.

Midplane/Symmetry Continuity

If your model is symmetrical then it will generally be quicker and more robust to model
half of it and then mirror the whole model - at least to the point where it becomes
asymmetrical.

To achieve continuity across the midplane:

All curves and resultant surfaces must be normal to the midplane.

Surface Classification

Surfaces within a model are often classified according to their aesthetic importance in the
final product.

The fundamental outer surfaces which are most prominent in a product are often classed
as the A surfaces - those which need most aesthetic consideration, ie. the top surfaces of
the mouse in your hand.

The surfaces which are generally hidden but may still be seen by the user, ie. the bottom
of the mouse, are classed as the B surfaces.
The C surfaces are then the internal, always hidden surfaces which need no aesthetic
consideration.

Model analysis
Do not build 'as is' - look for the separate patches used to build these
quilts. Identify which ones have been overbuilt and trimmed.
 Overbuilding then trimming/merging

Curvature

Spline – basically, a smooth curve with a constantly changing radius - discussion HERE

Complex surface - surface with a constantly changing radius

If we consider the best approximate circle radius that passes through a point on a complex
surface or spline curve, the reciprocal of the radius - 1/r - of this circle is the curvature of the
surface or curve at that point.

If a surface is nearly planar - flat - then a point on it will have a very large approximate radius -
1/r will give a low curvature.

If a surface is has a very tight bend in it then a point on it will have a very small approximate
radius - 1/r will give a high curvature.
In the above image:

Red line is the surface cross section or a spline curve

The yellow circles are the approximate radius at those points

The blue line with grey spines is the Curvature Plot - the longer the spine, the higher the
curvature, small radius - high curvature, large radius - small curvature.

Arcs or Splines?

Where possible, always use splines for complex surface sections.

Multiple arcs will give multiple patches in the resultant quilt with
only G1 endpoint/boundary relations.

Click image below for more info

Section Curvature - Splines and Surfaces

Always start with the minimum amount of control in a curve or

surface. The system as to adhere to your specified control
points/curve whether they are smooth or not. Better to allow the
system to find the smoothest path between minimum control
points/sections.
Spline curve creation and editing

Spline – basically, a smooth curve with a constantly changing radius - discussion HERE

Spline curves should be your default tool for sections underlying complex surface
forms. Planar spline are created in Sketcher (covered here), 3D spline are
created with Curve thru' Points or Style (ISDX) curves - see relevant sections.

Ending a spline - use the MMB to finish creating the spline

Where ever possible always start with a 2 point spline - see previous
section. In sketcher create a curve with 2 end points, set end
conditions to references, modify the spline shapes through the end
vectors.

 Select the spline

 Choose Modify from the Sketch toolbar
 either:
 Choose 'Modify spline using control points' from the
Modify toolbar - often referred to as a Control Polygon -
this returns you to interpolation point control was exited from
the Modify environment
 or;
  Choose to switch control to polygon mode to keep the
control polygon active when exited from the Modify
environment.
 MMB to exit Modify mode

The direction and length (weight or magnitude) of the end vectors

controls the spline shape. The direction of the vector shows the
direction of the curve end. The length of the vector dictates how far
into the curve that direction influences the curve shape.

Setting spline end conditions

Switching to control polygon mode allows you to simply apply

geometric constraints to the end vectors - Horizontal, Vertical or
Perpendicular are the most useful.

Curvature Continuity in Sketcher

The curve end condition can be set to Tangency - G1 or

Curvature Continuity - G2:

 activate the Tangency (G1) or Equality (G2) geometric

constraint
 pick Spline > pick connected Line/Arc
 A tangency 'T' or 'T' and 'C' continuity icon will show

nce you have set a tangency relationship from a spline to another

entity, this can be raised to Curvature Continuity - G2 - by adding
an Equality constraint to the connection;

 Tangency > pick Spline > pick connected Line/Arc

 Equality > pick connected Line/Arc
 A continuity 'C' constraint icon will show along with the
tangency 'T'

Boundary Surface Feature

Planar Surfaces - Fill, Trimmed

DO NOT create planar surfaces with a Boundary Blend. This functionality is for creating
surfaces with curvature in 2 directions - a blend in 2 directions. If you need to create a planar
surface then use the Fill function [Insert > Fill] to 'fill' a sketch or Trim/Merge or Extrude/Cut
an overbuilt or extruded surface.

A surface created by two or more edges or curves. Creating a boundary surface with two or
three boundaries is possible but can cause issues if you want to progress to a solid, initially,
always try and create your surfaces as 4 sided blends.

The functionality is similar to a simple Blend. The two pairs of opposite boundaries are
blended into each other through any intermediate sections. These two blends are then
'averaged' out to form a single surface.

A boundary blend does not have to be just 4 curves, there can be as many sections as
you like in each direction - a Quilt of patches. Collect the sections in the 1st Direction then
collect the chains in the 2nd Direction - see the next page for selection techniques
The 'corner' connection of the first direction curves to the second direction curves cannot
have a tangential relationship - the curve at the corner will then be travelling in the same
direction and will not satisfy the need for curves in two blend 'directions'.

If you want to set up boundary conditions (tangency, curvature continuity) in a new surface
with an existing surface then the surfaces have to have a common boundary - either use the
construction curve or the edge as the boundary for the new surface.

Construction and manipulation

Golden Rule No.1: All curves or edges to be used as your surface boundaries must be
robustly related to each other at the same level required in your surface boundaries.

Chain selection and trimming

Your surface boundary should consist of four boundary chains. It may then have internal
cross curve chains. Each chain could be a single curve/edge or a number of curves/edges
chained together.

Selection Techniques.

RMB [right mouse button] - when hovering over an element to pick it you can use the RMB
[momentary press, not press and hold] to toggle through all the selectable elements under
the cursor. This will also highlight part of a curve.

CRTL key - hold whilst collecting curves in one direction

SHIFT key - if one of the boundaries needs to be a chain of edge/curve elements then:

- select the initial 'anchor' curve/edge

- release the CRTL key and hold the SHIFT key

 - hover over the segment you you are working on to see the pop-up hint 'one-by-one' - left
click the curve again to change the selection method - keep hold of the shift key.

- select the segments you need for the chain. Remember you can right click to toggle
through the selectable segments

- return to the CRTL key to select the next curve in that direction

This seems a bit awkward when written down but is quite easy and quick once your used to it.

Curve end handles - The right click menu under the end chain handle allows you to trim the
chain length.

Boundary conditions

To set the boundary conditions where two surfaces meet, simply right click the condition
marker and choose the appropriate level.

If your boundary uses the curve rather than the edge then you will have to select the surface
to which you want to create the relationship.

Remember, a boundary relationship can only be as high as the level of the curves
which form that boundary.

Boundary influence

This example looks at the result of using multiple or single patches and the resulting boundary
influence
Construction and manipulation

Golden Rule No.1: All curves or edges to be used as your surface boundaries must be
robustly related to each other at the same level required in your surface boundaries.

Chain selection and trimming

Your surface boundary should consist of four boundary chains. It may then have internal
cross curve chains. Each chain could be a single curve/edge or a number of curves/edges
chained together.

Selection Techniques.

RMB [right mouse button] - when hovering over an element to pick it you can use the RMB
[momentary press, not press and hold] to toggle through all the selectable elements under
the cursor. This will also highlight part of a curve.

CRTL key - hold whilst collecting curves in one direction

SHIFT key - if one of the boundaries needs to be a chain of edge/curve elements then:

- select the initial 'anchor' curve/edge

- release the CRTL key and hold the SHIFT key

- hover over the segment you you are working on to see the pop-up hint 'one-by-one' - left
click the curve again to change the selection method - keep hold of the shift key.

- select the segments you need for the chain. Remember you can right click to toggle
through the selectable segments

- return to the CRTL key to select the next curve in that direction

This seems a bit awkward when written down but is quite easy and quick once your used to it.

Curve end handles - The right click menu under the end chain handle allows you to trim the
chain length.

Boundary conditions

To set the boundary conditions where two surfaces meet, simply right click the condition
marker and choose the appropriate level.

If your boundary uses the curve rather than the edge then you will have to select the surface
to which you want to create the relationship.

Remember, a boundary relationship can only be as high as the level of the curves
which form that boundary.
Boundary influence

This example looks at the result of using multiple or single patches and the resulting boundary
influence

Click the image below to enlarge

The above images show three different constructions - the first two have the bulge
constructed using two patches and the third has the bulge constructed as one patch with one
internal curve.

Two types of analysis are shown for each method - Gaussian and curvature spines.

In the first two models we have alternate 'leader' [parent] and 'follower' [child] surfaces. The
follower surface is constructed to satisfy the curvature continuity condition across the
boundary while the leader remains unchanged. You can see a sudden peak in curvature just
passed the boundary.

The third model is a single surface with an internal curve. The curvature flows smoothly
across the internal curve.

Therefore, create a quilt with as few individual surfaces as possible - the example at the
beginning of this page should be created as a single feature.

But.....do not take this too far. Unlike freeform surfaces, where you will see large quilts with
lots of dramatic changes in surface and boundary direction and curvature, with ProE you are

better splitting your quilts into areas which naturally group together. Mesh the surface to

make sure the UV lines aren't 'working too hard' - have dramatic changes of
direction/curvature.

Leader/follower Workaround

If you have to have a leader follower situation across a boundary and it cause a poor
continuity section across the boundary [as in first and second image above] then you might try
creating a ribbon surface on the boundary before creating the two surfaces and then using
this as the reference for the boundary condition.

The above images show three different constructions - the first two have the bulge
constructed using two patches and the third has the bulge constructed as one patch with one
internal curve.

Two types of analysis are shown for each method - Gaussian and curvature spines.

In the first two models we have alternate 'leader' [parent] and 'follower' [child] surfaces. The
follower surface is constructed to satisfy the curvature continuity condition across the
boundary while the leader remains unchanged. You can see a sudden peak in curvature just
passed the boundary.

The third model is a single surface with an internal curve. The curvature flows smoothly
across the internal curve.
Therefore, create a quilt with as few individual surfaces as possible - the example at the
beginning of this page should be created as a single feature.

But.....do not take this too far. Unlike freeform surfaces, where you will see large quilts with
lots of dramatic changes in surface and boundary direction and curvature, with ProE you are

better splitting your quilts into areas which naturally group together. Mesh the surface to

make sure the UV lines aren't 'working too hard' - have dramatic changes of
direction/curvature.

Leader/follower Workaround

If you have to have a leader follower situation across a boundary and it cause a poor
continuity section across the boundary [as in first and second image above] then you might try
creating a ribbon surface on the boundary before creating the two surfaces and then using
this as the reference for the boundary condition.

Merging and Trimming Surfaces

If you create separate surface features with a common boundary it may look like
there is a single boundary edge, there is in fact two edges occupying the same
position. These are two single sided edges - a surface only resides on one side of
the edge.

In the image below there are two surface features which have two patches each.
The green edges are single sided - a patch on only one side. The purple edges
are double sided - a patch on both sides.

The green horizontal edge across the middle is in fact two single sided edges in
the same place.
  One surface can be used to trim another
 A surface can be trimmed using a curve on the surface
 Two surfaces can be merged, removing any overlapping sections

Merge

 Ctrl select two surface quilts

 Merge
 Ctrl select further quilts if needed whilst in the feature - you
can Merge more than two quilts at a time

Depending on the nature of the chosen geometry and how it

intersects, the Dashboard direction arrows will flip which patches
are joined or trimmed.

Trim

A quilt can only be trimmed if there is suitable geometry interacting

with it - a second surface or datum plane intersecting it, a curve on
the surface.

Select the surface > Trim > select the trimming geometry
If you use the flip direction arrow on the dashboard rather than in
the graphics area, you can toggle to trim side A, side B or to keep
both sides as separate quilts. You can also use this toggle option
when using an Extrude to cut a surface.

Surface Fillets

A fillet can only be formed between two surface patches if the patches are part of
the same quilt and not if they are separate features. Merge the two features
then fillet the boundary. Select the edge to be filleted.

Solidify

The Solidify command will perform various operations dependent of the selected geometry.

A number of surfaces enclosing a volume can be used to form a solid - all the individual
surfaces need to be merged as a quilt first. An 'open' surface volume can also be closed by
the intersection of a solid which 'closes' the volume.

A surface can be used as a cutting plane through a solid - make sure you select the cut option
in the dashboard.

Thicken

In a similar way to a Shell, offset surfaces can be created from a

quilt to produce a solid.
The Thicken process will fail if there is geometry the system cannot
resolve - small, narrow, high curvature surfaces are classics to fail.

Use the preview button to force the system to try and build the
geometry, if elements fail it may then give you the option to exclude
the failed surfaces which you can handle manually.

3 sided surfaces

You will regularly meet situations where the skeleton which forms the boundary of your
proposed surfaces are comprised of 1, 2, 3, 5........ curves rather than the recommended 4.

You need to revisit [here] how a boundary blend surface is constructed before you can decide
how to deal with these situations.

If you create a surface with 3 sides [as above] you will have 2 curves in one direction and one
in the second direction. The pair of curves will converge at one end, at this point you are
trying to blend over a distance of zero.
This convergence will cause ripples in the surfaces near the convergence. This is OK if the
surface is not going to be thickened but may cause problems if you try and make the surface
solid. There could be alot of modelling between creating the surface and later on thickening it
only to then have to change the original surface and deal with the consequences.

Construction methods for 3 sided boundaries

Trim out the converging corner and replace with a 4 sided patch. Notice the shape of the trim
to make the UV isolines in the new patch blend as naturally as possible.

Try not to be constrained by visualising surface in their end form. Can the surface be
overbuilt and trimmed back.

Offset surface feature driven by sketch

The Offset function is another feature which has multiple uses depended on what geometry
you pre-select and what options you choose in the dashboard.
Select the surface you want to offset. If its the surface of a solid then select the solid then the
surface on the solid.

Edit > Offset

The default option is to create an offset copy of the whole surface. If you want to offset an
area defined by a [planar] sketch then you need to select the Expand option in the dashboard

Through Options you can then select or define the sketch which controls the offset area.
Consider whether you want the side surfaces to be normal to the sketchplane or the surface.

Note: You cannot use the text tool in sketcher for the offset sketch. If you want to use
standard fonts you will have to create the sketch using the text tool then create a second
sketch which traces the edges of the original sketch.

Level 3 Modelling

Advanced modelling
The emphasis at this level will be on good quality surfaces and
surface transitions and robust assemblies using a topdown design
approach

Boundary Blend Tweaks

Boundary Conditions

Curve End Adjustment

Set Boundary influences

In a one-directional blended surface, for boundary conditions

specified as Tangent or Curvature, ProE makes the side edges of the
blended surface tangent to the side edges of the references.

Control Points

If your boundaries are created from a chain of edges (arcs or

splines) then the resultant surfaces has to have multiple patches -
edges propagating from each chain junction - the Control Points.

If the boundary pair have differing numbers of Control Points then

the system needs to split the chain with fewer element to
accommodate the chain with more elements, sometimes the results
are not appropriate.

Sketcher - Convert Arc Chain to Splines

ISDX: Interactive Surface Design Extension

ISDX is PTC’s version of a freeform modeller which sits in Creo.

Skeleton curves, surfaces and surface deformation features exist
within a single Style feature. Although the Style feature has its own
feature tree and parent child relationships are formed, the
chronology of the features in the tree is not significant.
The interface can be viewed in single or four pane mode (below).
Four pane mode (icon in top toolbar) is most useful when
manipulating 3D curves which are tricky to visualise in from a single
view point.

The ease with which you can setup curve attachments and end
conditions, and the dynamic updating of all geometry as you
interact with curves on screen makes this module very powerful.
Unlike generic freeform modellers these relationships once set are
fixed and will update as related geometry is developed.

Most functionality can be found under RMB menus. Select or hover

over an entity to give appropriate RMB menus. Alt, Shift and Ctrl
are useful modifier keys with most functionality.

Curves

 Free – points placed arbitrarily in 3D space

 Planar – points placed on the active plane/planar surface
 COS – Curve on Surface – points stay within one surface
patch indicated by the first pick
Use Shift when placing a curve point to ‘snap’ to an existing entity,
also use shift to detach the point. RMB > pick soft point to toggle
through underlying entities. You can snap to a datum plane but you
may have to snap to its graphical boundary and then drag the point
to the required position. It can take a bit of experimentation to
choose the right reference which is appropriate for the required
end/boundary conditions.

MMB to complete curve creation and create further curves, MMB

again to return to select tool. MMB is generally a quick option to
complete or repeat operations in ISDX

COS across patches – as a COS is restricted to a single patch you

will have to think carefully about how you create a curve across
multiple patches, particularly if you want end conditions to adjacent
features. You could either; project a planar curve onto multiple
patches, or; create separate COS curves and connect the end points
across the patch boundaries.

Point Definition

 Filled circle - Free Point

 Empty circle – point attached to a curve/edge
 Empty Square – point attached to surface
 Cross – point attached to vertex or intersection point
 Yellow line - tangent bar
Point Attachment

In the above image, the curve in the right image needs to be G1 to

the two adjacent edges. Two issues to watch out for; ·

Don’t attach to the vertex at the end of the edge (X point marker –
left image below) – you cannot create a geometric (tangent in this
case) relationship to a point. ·

Make sure you attach to the edge and not the underlying
construction curve – you won’t form a loop for the surface. ·

Shift > attach to the edge > RMB > Pick Softpoint to ensure it is
the edge and not the curve. ·

Edit > drag the point (should be an open circle) to the end of the
edge to form a loop with the trimmed edges

Curve Editing and End Conditions

Dbl click a curve or use the Curve Edit icon to enter the edit
environment, simply drag the points to adjust the curve – all
connections will be maintained. Point > Point Movement and
used the nudge tool to move a point by controlled increments. RMB
menus to add or delete points.

Setting up tangency conditions on curve ends and surfaces is

fundamental to success in ISDX. Select the end point of a curve to
display the tangent marker, hover over the marker and RMB to
select a tangency condition – remember it has to have an
appropriate relation to establish an end condition. Dragging the
length of the end marker changes the influences into the curve.

 Hold shift whilst dragging a connected point to disconnect it and

reconnect elsewhere
 Also use alt and alt+ctrl to constrain movement
 Trimming - COS cannot lie across patches - planar curve - project then trim
 Shift+alt to extend curve - add new point from end

Surfaces
Follow the same principles for creating surfaces in ISDX as in the
core ProE functionality – curve skeleton structure, blended 4 sided
surfaces, 3 sided surfaces etc. Boundary selection is different:

Boundary Blend Surface

 ctrl pick the 3/4 boundaries (3 sided surface issues still

apply) – selection order is irrelevant
 if one boundary is a chain then ctrl pick the first element,
switch to shift to pick the chain, return to ctrl to select
further boundaries
 internal curves are then collected after moving focus to the
Internal Chains window

Blended Surface

 Single primary curve in one direction, single or multiple curves

in second direction
 Select primary curve
 RMB > Cross collector > select cross curve[s]

Lofted Surface

 Ctrl pick multiple, unattached section curves in one direction

Surface Tangency

By default the system will establish boundary conditions according

to the underlying curve conditions:

 position – common boundary - G0

 tangent/normal – G1
 curvature continuous – G2

To edit the surface, double click the surface or RMB > edit
definition in the ISDX model tree. Either RMB or pick the middle
of the boundary marker to toggle between position (G0), tangent
(G1) and curvature continuous (G2) connection – if the controlling
curve conditions allow.

The arrow points from the leader to the follower surface, the
follower surface changes shape to satisfy tangency conditions.
RMB > Flip Leader on the arrow end allows you to (if relations
allow) reverse the leader/follower order - this can have a significant
effect on the form.

Surface Trim

Use of MMB makes the surface trim operation very quick and easy
  start the trim tool
 pick the surface to trim > MMB
 pick the trimming reference – curve[s], surface, plane > MMB
 pick the portion of the surface to delete > MMB

Direct surface edit

This tool can be used to edit surfaces for purposes of general

modelling as well as make subtle tweaks to smooth out problem
areas. The history of surface edits is maintained during future
regeneration, so if the parent surface is modified, the surface edit is
reapplied to the surface during regeneration.

 Adjust the number of rows and columns for coarse or fine

adjustment
 Define how you want the points to move relative to the
surface – normal to the surface, normal to a plane, free, etc.
 Select individual points, Ctrl pick multiple points, select whole
rows or columns.
 Avoid distortion of surface edges - RMB menu on edge control
lines and lock the edge.
  Use the dashboard Nudge controls to incrementally move the
control points
 Experiment with the Filter to change the characteristics of the
distortion away from the dragged point

Hiding ISDX Elements

You can RMB > Hide any ISDX feature whilst creating/editing the
Style feature but this will not stay 'fixed' when you have exited the
feature.

Layers - to hide ISDX surfaces - outside of the Style feature >

Layers > RMB > new layer > change the Selection Filter (top
right of graphics area) from Smart to Quilt > select ISDX surfaces
to add to the layer > hide the layer

ISDX Style Trace Sketch Function - reverse engineering

Take some photos of an existing product or scan your sketches, you

can then use the images as the basis of your initial reference
curves. Don't put any geometry in this feature as you will have to
suppress it to hide it.
Whilst in a Style feature:

 Drop down menu Styling > Trace sketch

 Select one of the existing planes or use the plus sign to add
an additional plane
 Search for you image file

Fit

Drag the two yellow bars to align to the the two reference points of
a known distance - say the two axle centre on the image of a bike.

Input the actual distance and click fit

The bitmap will be scaled

Expand the Properties functions at the bottom of the Trace Sketch window to
control your image

To set up 3 standard views, you may have to create a mirror image

of your bitmap as it only applies to one side of the plane and there
is no flip option.

Photo tips:

 put a ruler in the image for easy scaling

 use maximum zoom to avoid wide angle distortion - more
zoom more isometric
 leave plenty of space around the subject and crop the image -
there is more distortion at the edges of the image and you
don't need a high res image

Scoops, Bulges and Split Surfaces

Split or tearing surfaces are large scoops or bulges that merge with the main surface on two
or three of its sides in a fluid manner, indicating that they are parts of the main surface. The
remaining boundaries, are created above or below the main surface giving the impression
they are split or torn from the main surface. Such surfaces are often used to define aesthetic
features.

A typical split surface is shown in the following figures

The challenge in creating these features is the construction of the tangent/curvature boundary
and its underlying construction curves. This requires a good understanding of the 3D form, a
clear statement of your design intent and identification of the boundaries.
If you are working from a sketch make sure you draw all the surface boundaries and show
their conditions. If you are reverse engineering a product, draw the boundaries directly onto
the product and again, indicate their condition.
Click on the image to enlarge

The above image shows a number of surface features which have tangency to the parent
surface and could be interpreted as having issues of 3 sided surfaces and convergence. The
right hand image shows the construction curves for these surfaces.

The tapering groove and the elliptical bulges are based on simple rectangular surfaces. All
the curves and surface boundaries have tangency to the parent surface.

The top and bottom features are rectangular peel surfaces with fill strip surfaces. The top one
has tangency on 3 edges and the bottom on one edge.
5 Sided Surfaces

One of the trickiest scenarios to overcome is when your form suggests a patch which does
not obviously suggest how it can be broken into multiple 4 sided patches or overbuilt and
trimmed.
1. Initial curve set – simple sketched
datum curves - ensure you have curve
end normalcy where needed
 2. Construction curve to enable initial 4
sided – curve thru’ points or ISDX free
curve - again, consider end conditions

3. First 4 sided – boundary blend or

ISDX

4. Trimming curve – ISDX COS,

projected curve or simply extruded
surface cut. Make sure the curve is
sympathetic to its opposite blend curve.

5. Trim initial surface

6. Second 4 sided surface – some

tweaking of the trim curve is likely to
be needed. If you can’t create
appropriate boundary conditions you
will have to revisit your construction
curve end relationships and end
conditions

Surface and Section Analysis

Much of the work in creating good surface models goes into fine tuning the curves and
surfaces once they have been built. There are various formal analysis tools available but
don't forget to use the most important one - your eyes.

Selection
The selection filter - bottom right of window - defaults to Smart or All. Is this mode you will
have to Ctrl select the individual patches you want to analyse. Change the filter to Quilt to
select whole quilts.

Visual analysis

Always make a visual analysis the first level - ultimately, that's all the consumer will do. To
make a good visual analysis of your surfaces need to be a dark, high gloss finish with a
directional light.

Through the render toolbar, turn off the default ambient light. Change the part colour to a
dark colour with high reflectivity - there is a suitable colour already set up in the appearance
window.

Also turn off your datum curves so they do not hide edges - there is a Mapkey setup to turnoff
- F10 - and turn on - F11 - curves.

Zebra stripes

Simulates a mirror finish on your part in a black and white stripe environment. These stripes
are then reflected across boundaries and you can visually check continuities.
Section analysis

This tool with analyse the curvature of multiple cross sections. We are looking for a smooth
change in curvature along the section.

icon in analysis toolbar

Ctrl pick the surfaces to be analysed

Select a planar surface or datum plane to which the cross sections will be parallel.

Change the number of sections and drag the position of the first and last section.

Adjust the scale of the curvature spines.

Rhino

We have some licenses on Rhino in XX001/2 and I shall endeavour to learn how to use it for
starters and put post resources as I come across them.

http://www.rhino3d.tv - Quicktime vids

http://www.rhino3d.com/tutorials.htm

Useful tools

Rebuild Surfaces - allows primitives to be deformed through specified numbers of control

points U and V

'Naked' edges - to export a model with mass properties, ie. a closed, watertight volume, it
needs to have no single sided edges or cracks or slivers.

Edit menu: Object properties - an open quilt will show as an Open Polysurface

Analyze menu: Edge tools > Show edges

FAQ Closed Solids - http://en.wiki.mcneel.com/default.aspx/McNeel/FaqClosedSolids.html

FAQ Tolerances - http://en.wiki.mcneel.com/default.aspx/McNeel/FaqTolerances.html

Shortcut keys
F10 - turn control points on

Useful

Surface from Network of Curves - give tan options

Match Curve tool - to attach tangent

Assemblies

If the product your model represents exists in reality in several parts assembled or moulded
together then it is most appropriate that these parts are modelled as separate part files which
are then brought together to represent the end product - this is an assembly.

The assembly file [extension .asm] is a separate Creo file. All that it contains is the name of
the parts files, where they are stored and positional information about how they fit together.

It is important to remember that the part files are not transferred [or stored in any way] to the
assembly file. What you see is simply an image [instance] of the part file in its current state -
if you open the part file and change it then the assembly will change. The part file instances
in the assembly file are referred to as Components.

The assembly file is associated to the part files - it cannot exist with out the parts files.

Assemblies
Key terms:
Constraints
Degrees of Freedom (DoF)
Base part
Align
Mate
Insert
Coincident
Offset
Oriented

File Management

Good file management becomes absolutely in the success of your assemblies. As

you create new files your are creating relationships between those files -
associativity - it is important you keep track of where those files are going.

Golden Rule: Keep .asm files and all associated .prt (or sub assembly files) local
to each other - in the same folder

The simplest working folder would be on your U:/ space, but currently IT Services
are not able to accommodate this so you will need to work from the hard drive if
you are creating new files and need to maintain associativity.

 Have all your files in a project folder

 Put that folder in the Working Directory - follow the shortcut on
TeachDoc for LDS003 or LDS011
 Through the Model Browser tab in the Model Tree, RMB and set that
folder as your Working Directory
 All assembled part files MUST stay in the same folder as the .asm file
 DO NOT change the name of any of the part files once they are in an
assembly

To begin with, we shall bring different parts [or copies of the same part] into an assembly file
and position them relative to each other with constraints such that they have no degrees of
freedom [DoF] – that is they cannot not move in X, Y or Z or rotate around the X, Y or Z axis.

See the Simulation section for creating assemblies with DoF which enable mechanism
simulation and analysis.
+ve and -ve

All datum planes and surfaces have a +ve and -ve side. The positive side of a datum
plane is brown, the negative is black. The positive side of a solid surface is the outside - the
side you can see.

The positive direction is therefore normal to the surface away from the positive side.

Tip: When you first bring a part into the assembly, press the Ctrl and Alt buttons together
and use MMB or RMB to move that part to the approximate position and orientation relative to
the parent part.

Keep it simple and logical

Think about how the components might be assembled in reality, which references would be
aligned - screw holes? edges? cylindrical axis? If you run out of fundamental geometry then
use Datum Planes

A rule of thumb is; you need at least three constraints to place a part. There are exceptions
to this rule - eg. aligning two axis which are perpendicular to each other will constrain a part.

Think about your references

To begin with, generally try and constraint a part to only one other part – this will make
modification of the assembly a lot simpler. If you are putting a wheel in a pair of bicycle forks,
the wheel should only be related to the forks, not to the frame or the planes in the assembly
environment.

To test how robust your assembly is try moving the base part and see if everything follows it
or if the assembly fails.

Any squares next to the component name in your model tree mean a part is not fully
constrained. A small square over a large square shows that that part is constrained but its
parent isn't - therefore it still has DoF via its parent. If you can move or rotate a part using
ctrl/alt middle/right mouse then it is not fully constrained. A component which is not fully
constrained is referred to as 'packaged'.
All surfaces and planes have a positive and negative side. Any cylindrical surface (hole,
protrusion, etc.) usually has an axis.

The process

Choose the Add Component icon (above) > select (Dbl click) the
component to add to the assembly

Default Constraint

Be logical about which part of your product to assembly first - if you were assembling a car
you would probably start with the chassis and not the steering wheel. This is the base part.

Firstly, make sure the base part is fully constrained. The base part can be simply placed by
using the default placement icon – this will align the default planes [xz, yz, xy] in the part to
the default planes in the assembly environment.

Bring in the Component > RMB in the grahics area > Default Constraint

Primary constraints - Constraint Type

This is the first element of the constraint description.

Once the base part is assembled you need to think carefully how the
subsequent parts relate to it.

Automatic Mode

By default, without entering the Placement window (above), the system in in

Automatic constraint mode - simply select two appropriate reference and a
constarint will be created according to the nature of the references - planar or
cylindrical surfaces, axis, etc.

Continue selecting references and new contraints will be automatically created.

Align – positive/negative side of the aligned surfaces or planes facing in the same direction.
Two axis coincident - in the same place.

Mate – positive/negative side of the aligned surfaces or planes facing each other.

Insert – cylindrical surfaces concentric – the same as aligning two axis but sometimes there
is no axis.
Secondary constraint - Offset

The offset element of the constraint controls how far apart the reference surfaces or planes
are.

Coincident – touching each other

Offset – at a specified distance from each other

Oriented – satisfying the primary constraint (mate, align) but floating. Their distance apart is
dictated by another constraint, maybe the alignment of an axis.

Angular offset

If you want two parts at an angle to each other;

Align the appropriate axis

Constraint the position along the axis

This leaves one degree of freedom - rotation around the axis

Use crtl+alt and MMB and rotate the parts to approximately the correct angle

Within a new constraint, select the two surfaces/planes which set the angle [need to be
parallel to the axis]

An angular offset constraint will be generated.

DO NOT USE THE ‘FIX’ CONSTRAINT – this will simply hold the part in its current position in
the 3D environment but will not create any relationships between it and the other parts. This
constraint is used for temporary placement of a part.

Using this constraint WILL lose you marks in your assignments.

Constraint Conflict

Take care not to have two constraints controlling the same alignment.

In the above example, the cylinder axis is aligned with the hole axis. The rotational angular
position of the part is set by the alignment of the the flat at the top of the cylinder with the flat
in the top of the hole. If the the surfaces were set coincident then there would two constraint
trying to position the vertical height of the part - one would be pulling against the other.
This might be OK as long as the dimension are compatible, but if one of the dimension
changes then the coincident constraint cannot be satisfied and the assembly will fail. The
constraint for the parallel alignment needs to be simply oriented - parallel but floating.

Sub Assemblies

Sometimes it is easier [or more logical] to manage a product by organising some parts into
separate assemblies and then assembling those into the top assembly. These are referred to
as subassemblies.

In the above example the petrol drill is split into many logical subassemblies and sub
subassemblies!

Choosing appropriate, robust references when bringing in a subassembly is important. Think

about it logically, it is likely that you will use references in the base part in the subassembly to
connect to the relative part in the top assembly.

Assembly references must be considered very differently when using a top down design
approach - see the Bottom Up or Top Down section.

Patterns

Any assembled parts can be patterned in the assembly - linear, radial, reference or fill.

In the example below the bolts form a reference pattern - they are following the patterned
hole in the part file. In this setup you would need to make sure the first bolt is assembled to
the original hole.
Explode States and Cross Sections

View manager

The view manager combines various very useful tools which modify how a model or assembly
is displayed. Various different display states and effects can be saved and activated at any
time to assist visualisation of the project.

Explode states
'Exploding' an assembly does not effect the applied constraints, it is simply a temporary,
controlled positioning of the components to enabled easier visualisation of the separate parts
and how they fit together.

View Manager > Explode tab.

 Use the New button to create a new explode state

 RMB the Explode State > Edit Position to control the relative position

 The explode position window will first require a reference which controls the direction
in which a part will be dragged - the default is to simply pick an edge or axis.
 Then choose the part to be dragged and drag it to the required position.
 Right click and choose Set Active to enable a listed explode state
 Right click and choose Explode to deactivate all explode states and return to the
constrained state

Offset Lines

In the image at the top of this section there are blue Offset Lines which indicate how parts fit
together. These are creating by choosing the Offset Line icon.
You have to select the from-to reference and the direction the line travels. An example being
a cylinder being aligned to a hole. You would choose the axis or the cylindrical surface in the
cylinder, you may have to experiment with which geometry you select to get the line direction
right.

Once you return to the xsec List you need to RMB > Save the changes to the
explode state.

Cross Sections [xsec]

Removing part of the project at a defined cutting line can allow us to better visualise internal
detail and particularly how assemblies fit together.

For an assembly, make sure you have an assembly datum plane which defines the cutting
plane.
 View Manager > Xsec > New

Choose your cutting plane.

Right click and Set Active to activate a xsec in the list.

Right click and Visibility to show cross hatching

Edit > Redefine > Hatching to change the cross hatching style - spacing, angle, etc.

Dynamic X-sec

A simple dynamic X-sec can be created through

View > Display Setting > Visibilities

Use the Clip slider to section the part parallel to the screen.

You will need to be in shaded view.

View > Display Settings > Model Display > Shade

Untick capped clipping to stop the sectioned face showing in red

Top Down Design and Data Sharing

Bottom Up or Top Down Design Methodology?

Most projects will involve individual part files brought together in an assembly. In
our introduction to assemblies we looked at bringing existing part files into an
assembly environment. Any interfaces between parts (e.g. hole centres, mating
edges) were considered individually at the part level. If any changes were made
in one part it is only through a good awareness of the implications of those
changes that we ensured the parts still fitted together in the assembly.

This is referred to as a Bottom Up approach to designing. In reality we see a

product as a whole, an assembly of parts, from the ’top’ down. Two key methods
to move to a Top Down design approach are;

 creating and modifying your models in the assembly

environment and directly referencing geometry from other
parts or the assembly
 importing geometry or whole models from a 'master' model to
a part file maintaining associativity to the parent part

Part Activate

Right click part name in Model Tree > Activate

You are now in part mode but with the assembly still visible and available to
reference as you create features and modify your model. In the speaker example
below, the dimensions and position of the power and volume knobs are
controlled by the speaker body.

The part files were created in the assembly and assembled with the Default
constraint, the features are then created relative to the axis and faces in the
speaker body. Therefore if the speaker body changes, the knobs change and
clearances etc. are maintained. The knob diameter is controlled by a clearance
dimension from the speaker body which is a sketch reference in the revolve,
along with the axis and the end face.
Proceed with caution – as soon as you create reference across models you need
to think very carefully about modifying or delete associated files – references can
start falling over and solving issues can become problematic.

Skeleton Models

If we look at the relationships and interfaces between the different elements of

our product, the Design Intent, and construct those at the assembly level as a
basis for our part design then the parts will always follow this assembly
framework or skeleton. This framework could simply be as simple as a few
reference points and a couple of sketches created in the assembly file. The
skeleton model can be a formal Creo Skeleton Model or simply an ordinary part
file assigned as the skeleton model.

Creo Skeleton Model

A formal Creo Skeleton Model is created via the Create a component icon in the
assembly file and is insert at the top of the model tree. It has a couple of
immediate advantages:

 they do not show up in the BOM

 they do not contribute to mass properties

Therefore they can be a ‘transparent’ framework part on which to construct your

geometry.

Modelling in Assembly Mode

Working on your Part files (or Skeleton models) from within the assembly allows
you to work on parts ‘in context’. You can directly reference to other parts and
the Skeleton model and you can generally visualise the whole product.

Use the Create a Component icon on the right toolbar to create new part files as
your product develops. If your part is to be built on references from other existing
parts then simply assemble it using the default constraint placement, its
position in the assembly is now controlled by the existing parts as it would be in
reality.

Right click on the model name in the Model Tree and choose Activate. The
interface is now in standard part mode but all the other assembly parts are
shown. Right click and Activate the assembly name at the top of the Model Tree
to return to assembly mode.

Parent Child Relationships and Circular References

Consider very carefully any references you create across parts in assembly mode.
If you activate a part earlier in the model tree, all the later parts remain in the
assembly. Make sure you do create unsound or circular references to child parts.

External References

Another very powerful method utilised in a Top Down approach is to reference

external geometry to the current model. By bringing an image of specific
geometry from one model into another we can build features (and maintain an
associative relationship) based on that parent model. This does not have to be
undertaken in the assembly.
Two significant features to be considered are Copy Geometry and Merge Part.

External Geometry Example

If you consider the example assembly below which is the handle and grip section
of a power drill casing.

 create drill_grip.asm
 created New Component drill_grip_skel.prt as a skeleton
model
 created New Component case.prt
 created New Component grip.prt
 activate drill_grip_skel.prt, create reference surface and
curves
 activate case.prt, import surface and curves from
drill_grip_skel.prt as Copy Geom feature
 thicken surface, create offset pocket for grip, fillet edge
 activate grip.prt, import surface and curves from
drill_grip_skel.prt as Copy Geom feature
 create offset curve for grip clearance, trim surface
 thicken grip, fillet

If I want to change the form of the handle I make changes in the skeleton model,
these changes will then migrate through any associated models, in this
example, the case and grip parts. The ‘master ‘ model does not have to be a
formal Creo skeleton model, any part file could be the source for the driving
geometry.

Copy Geometry Method

 Open the part file independent of the assembly

 Insert > Shared Data > Copy Geometry
 Deactivate the Published Geometry Only button
 Click on References
 Use the File Open icon to find your reference model
 Decide how you are going to align the reference model in the
current model through the placement window – generally use
the Default constraint
 Click in the Surface Sets, Chain or References window
dependent on what geometry you want to copy from the
external model.

If the reference model is already open then through the Window drop down menu
go to that model window, otherwise a window will open showing the external
model. Resize and move the window out of the way and leave it open until you
complete the process. Select the geometry you want to copy.
Merge Part

Insert > Shared Data > Merge/Inheritance > find the reference part and
assemble appropriately

This process allows you to import an image of a whole part into the current part
file and maintain associativity.

Modelling in Assembly Mode

You can further develop your model by performing operations in the assembly file. These
come in two catergories:

Operations which exploit the relationship of parts in the assembly but have an effect at the
part level, and,

Assembly operations which will only show at the assembly level as they would in reality.

** You could have issues if all parts are not fully constrained **

Component Operations*

Edit > Component operations. Modelling which has an effect at the part level referencing
the intersecting volumes of parts.

Cut Out - cuts one part with another. Multiple parts can be selected.

Merge - merges one part into another.

Options:

Reference—References the second part to obtain its information. When the referenced part
changes, the merged or cut out part changes.
Copy—Copies all the features and relations of the second part into the first.

Assembly Features

In a manufacturing environment many operations are performed to parts once they are
assembled, eg. drilling holes, machining surfaces. It is important to remember that although
ultimately these features will change the shape of the part they do not exist at the part level.
therefore do not detail them in a part drawing, detail them in the assembly drawing. Modelling
features can only subtract material.

Assembly Features may be either Datum entities (Axes, Planes, Points, etc.) or subtractive
solid geometry (Holes or Cuts). All the normal functionality is available - extrude, revolve,
sweep blend, etc.

* Boolean Operations - you may see reference to boolean operations in generic CAD
discussion - union/merge, difference/cut, intersect. See definition here.

Model Analysis
Useful Tools

Global Interference will show any overlapping volumes in an assembly

Analysis > Model > Global Interference

Mass Properties will give you the volume/weight of a component or assembly.

The figure for volume is likely to be shown as an exponential figure in the modelling units.

In the example above VOLUME 8.5010447e+03 MM^3 , move the decimal place plus 3
places to give 8501.0447 MM^3. Remember to convert this figure if you need different units:

1000mm^3 = 1cm^3 8501.0447mm^3 = 8.5cm^3 [approx]

Engineering drawings – views

We create an engineering drawing of our model to formalise its parameters, communicate its
form and parameters and to archive the model.

What makes a good engineering drawing?

 Plan the sheet layout to best communicate the part

 Maximise the view scale to fill the sheet

 Use half view for symmetrical parts to save space

 Use section views to show internal detail

 Check all dimensions for clarity and ambiguity

 Always ask the question – “will someone else be able to visualise the form?”

All model views in the drawing file are associative, ie. there is no ‘linework’ stored in the
drawing file, each time you open the file the views are recreated according to the current
model version. If you change a dimensional value in the model or in a view, the system
updates other drawing views accordingly.

Remember; keep the .prt file and the .drw file together and do not change the model name.
If you do, the regeneration process will fail because the system cannot find the model file as
originally specified.

All drawing created in the Department should conform to BS8888. It is up to you to ensure
your ProE drawing conforms and achieves maximum clarity by manipulating the line work and
detailing and by changing the drawing setting file BS8888.dtl [File > Properties > Drawing
Options]

Creating a Drawing
When you open a new Drawing file [.drw] the New Drawing dialog box will open.

 Select the associated model

 Select the Empty with Format option – this applies a border and table

 Browse to find the format [.frm] file your after – A3/A4, landscape/portrait

Fill in the table information as you are prompted

Sheets

An engineering drawing isn't necessarily a single sheet of paper - or virtual sheet in the CAD
file. If more views are needed to communicate the part than can fit, at a suitable scale, on
one sheet then add sheets to the engineering drawing.

Insert > Sheet - you will be prompted to fill in the table as you were on the first sheet

The sheet list will then become active in the Drawing toolbar to switch between sheets.

Adding Drawing Views – [RMB menu]

The first view must be a general view. Use the Drawing View dialogue box to set up your
first view.

Your first view will probably be an orthographic view. Either use the list of saved views [from
the model] to set its orientation or orientate the view manually using the Geometric
References or Angles options.

Make sure you set a view scale to make best use of the sheet area.

Double-click a view to change its properties.

Other views such as, Detailed views, should be added through the Insert > Drawing View
drop down menu.

Types of Views

The primary view types available in the VIEW TYPE menu (illustrated in figure below) are:

 General – A view that you orient and is not dependent upon any other view for its
orientation.
 Projection – An orthographic projection of an object as seen from the front, top, right,
or left. First or third angle?
 Auxiliary – A view created by projecting 90 degrees to an inclined surface, datum
plane, or along an axis.
  Detailed – A view that you create by taking a portion of an existing view and scaling it
for dimensioning and clarification purposes. The boundary for the detailed view can
be a circle, ellipse (with or without a horizontal or vertical major axis), or a spline.

Click above image for bigger picture

Specifying How Much of the Model Is Visible

Using other options in the View Properties > View Type window, you can specify how much
of the model is visible in the view, as shown in the next figure.

 Full View – Shows the entire model.

 Half View – Shows only the portion of the model on one side of a datum plane.

 Broken View – Removes sections from large objects between two points and moves
the remaining sections close together.
 Partial View – Shows only the portion of the view that is contained within a boundary.
Adding a Cross Section

A cross sectional view is often needed to clarify internal detail – remember, never dimension
hidden detail, dimension the cross section. A perpendicular datum plane in the parent view is
used as the ‘cutting’ plane to allow a projected view to be showed in Cross Section [xsec]

To show the view as a cross-section, use the View Properties> Sections window options.
Either pick an existing xsec (which should be created in the model file - see HERE) or
create a new planar section.

Adding section arrows

Arrows are needed in the parent view to show the position of the cutting plane. Pick the xsec
view > RMB and choose add arrows > choose the view to which to add the arrows.

Adding a Detailed View

 Insert > Drawing View > Detailed View

 Pick a point on the part to show the centre of the detailed area

 You are prompted to draw a spline curve to represent the extents of the detailed area

DON'T start the spline tool from the sketch toolbar, just start picking points to show

the area.

 Middle mouse button to finish the spline

 Pick a position to place the view

 Change the scale accordingly

Isometric View

An isometric view can help us better visualise the 3D form. Use the orient view icon in the
part file to create an appropriate view or the view orientation area of the view properties
dialogue box to create your view. Rotate around the vertical axis 45 degrees, rotate around
the horizontal axis 35 degrees.

Videos
General orthograpic view - HERE

Isometric vew - HERE

Cross Section (x-sec) view - HERE

Detailed view - HERE

Line display

The settings wireframe, hidden line, no hidden line or shaded will affect the way your view are
displayed. Showing hidden detail is the preferred option, but if this makes the view
unreadable because of an extreme amount of internal detail then use no hidden line – make
sure you are consistent in any associated views

The line display setting can be controlled independently within each view through the view
properties window. Isometric views are generally not shown with hidden line detail, their main
function is to show the general form.

Multiple parts on single sheet

If you want to split your sheet into areas and details multiple parts then:

File > Properties > Drawing Models > Add Model

Then use the Set Model option to switch active models. Make sure you split up your sheet
and have a details table for each model.

Multiple Sheets

If you cannot include enough adequately sized views on a sheet to fully explain your model
then add sheets to the engineering drawing:

Insert > Sheet

Fill in the table info as before. Use the box in the top toolbar to switch between sheets.

“wysiwyg”

What you see, is what you get – your file will print as it is shown on screen. Turn off display of
reference geometry [planes and csys], switch to hidden line. Always do a test print and then
fine tune the drawing. Although hidden lines show in grey on the screen they will print as the
standard dashed lines.

Watch the ProE print defaults. When you hit the print icon, the system should be

configured to print ‘Full Plot’, that is, 1:1. If it doesn’t then your scale will be incorrect.
Change the setting in the ProE print window – Configure > Model > Full Plot

Show the associativity between the drawing the and the model file.

If you open and modify the file to which your drawing is associated and then regenerate the
drawing file it will be updated according to those changes.

Once you have applied dimensions to the drawing these can also be used to change the part
file.

Deleting unwanted lines

Common situation is when you have a mirrored part with normalcy across the symmetry plane
or merged surface patches at G2/curvature continuous - this will create tangent/patch edges
which shouldn't be there as there is no abrupt change in radius.

Also, stray, random lines can be created if the system cannot fully resolve the geometry.

View > Drawing Display > Edge Display > Erase Line

Engineering drawings – detailing

Once we have some views which best communicate our form, we need to show the physical
size of the elements in that form and, by carefully deciding how we dimension the form,
communicate our ‘design intent’

Capturing design intent – feature dimensions and feature position

Consider the above image. If I was communicating this part to a third party part of my
description would describe a rectangular pad in the middle of the angled surface and two
holes drilled into the rectangular pad.

The rectangular pad is a feature [not a ProE feature] and the holes in the pad are a feature.
Each of these features have their own dimensions to describe them and then dimensions
which place them relative to their parent feature. Feature dimensions and feature
position.

The pad is placed on the angled face a distance from the side wall and a distance from the
bottom edge. It is then x wide and y high. If its position changes I don't want its size to
change.

The holes are x and y distances from the edges of the pad. If the pad moves the holes need
to stay in the same place on the pad.

These two last statements are my Design Intent. This design intent needs to be captured in
my dimensioning scheme.
BAD

Consider the above dimensioning scheme. What would happen if I changed the 7 and 8
dimensions to move the pad down and across slightly?

The pad size would change and the holes would move relative to the pad.

The above scheme will also cause tolerance accumulation. Say I have a general tolerance
of
+/- 0.1. The pad width is controlled by the 7 and 39 dimns. Therefore if the 7 was minus and
the 39 was plus [or visa versa] the pad feature width is +/- 0.2
BETTER

The above dimensioning scheme better captures my design intent. If I change the 7 and 8
dimensions to move the pad, the pad size will remain constant and the holes will remain in the
same place relative to the pad.

The above scheme still does not address what seems to be a symmetrical design intent or the
holes centres. In this situation we could dimension from a datum plane which would maintain
the holes centres and their position relative to the pad.

Rule: Dimension the feature and position the feature

Conflicting dimensions or over constraining

This drawings has too many dimensions - changing one dimension will conflict with the others

Apply all the same rules from your manual drawing practice - some common issues
are:
  always show axis
 dimension as diameters where appropriate, not the default radii
 don't show hidden line in GAs or isometric views, but always in part drawings
 accepting what your given by the CAD - don't be lazy!
 nonsense dimensions - see Design Intent

Axis

Before we can start dimensioning any arcs we need to show axis.

Select an individual view or Ctrl select multiple views

RMB menu > Show Model Annotation > pick the Axis tab >
select individual axis or use the Tick All button

Show Model Annotation icon in the Annotation menu

will also access this window

Driven Dimensions

Creation is similar to creating dimensions in Sketcher

LMB to select the elements, e.g. length of a line, distance between
two lines, radius of an arc

MMB to place the dimension - placement can determine which

dimension is created, ie. inside or outside angle

Drag the projection lines, dimension lines and dimension text for
best clarity

Picks

 pick a straight line to show its length

 pick two parallel lines to show the distance between them

 pick two non parallel lines to show the angle between them - MMB pick position for

inside or outside angle

 pick an arc to show its radius

 pick an arc once, pick it again, then MMB to shows its diameter

Hint: If a radius or diameter dimension fails or is created with an X

and Y element then go back and make sure the plane of the
diameter is parallel to the screen – its axis is normal to the screen.
It only has to be a fraction of a degree off parallel and the circle
becomes an ellipse.

Dimension Text

Formatting Dimensions
Make sure your dimension are a suitable height and font style for maximum clarity.

Either; pick the individual dimension, RMB > Properties > Text Style tab

Or; drag a box around all the dimensions, RMB > Properties > Text Style tab
The Defaults are driven by the .dtl config file - in our case, BS8888.dtl in the
working directory

Select dimn. > RMB menu > Dimension Properties > Properties >
Name - this shows the dimension (from the model) which is driving the
dimension text in the Display tab. By default you will see @D in the Display text
window. You can simply add text before or after @D to modify the dimension text.

You can control the entire text label by replacing the @D with @O to overwrite
the default text. Put in your own text after the @O

Notes

Notes add additional information to the drawing sheet either floating

on the sheet or attached to an entity via a leader.

Caution: if you put dimensional information in a note manually it is

not associative to the model - if the model changes you need to
remember to manually update the note. We can exploit the power
of the parametric system to link notes to model dimensions.

To find a dimension name - in the model file RMB > Edit on the appropriate
feature - this will show the dimension associated with that feature. From the Info
drop down menu > Switch Dimensions to show the dimensions name rather
than value. This is the identity which can be used in notes and dimensions text.
In the example below, a note to detail the hole is neater then applying the dimensions to the
section view. The note is associated to dimensions in the model. Insert &[dimn name] (see
above) in the Note text box to insert the dimension in your text and remain associative.

Dimensioning to a symmetry plane

If a part is completely symmetrical then you can robustly communicate the design intent and
save space by using a half view and and dimension from a centre line.
You will need to have a datum plane as the symmetry plane. Right click and properties for
the plane in the part file. Rename the plane CL and set to the middle Type setting. This will
allow you to use the plane for dimensioning in the drawing.

Create the dimension in the full view and then change the view to a half view.

General Assembly Drawings

Create your drawing by the usual process;
New > Drawing > Empty with Format > [Browse to select appropriate
Format file]
If prompted, click OK to specify No Combined State.
Remember;

 No hidden line in views

 show axis where needed
 No part feature dimns in views, but...
 .....you can have component position dimns or assembly level feature
dimns
 xsec views will give best detail of assembly interfaces

Bill of Materials - BOM

Once you have a General Assembly drawing of your assembly file you will need to create a
table which lists all the parts in that assembly and some information about them. This is a Bill
of Materials (BOM).
Add and define a table for the BOM

We could create a table and manually input the information describing the assembly but this

would have to be updated manually and does not exploit the associativity between the

assembly and the GA. We can create an associative link between the table and the assembly
using a Repeat Region.

To create an automatic BOM in ProE we need to:

 create a table
 define a simple repeat region
 enter the report symbols
 update the table
 add BOM balloons

Creating a Table to contain the BOM

Use the Insert Table icon in the top toolbar then [for a descending table in the top, right
corner] from the Menu Manager choose Descending > Leftward > By Num Chars

Select the upper, right corner of the drawing sheet border as the start position of the table.

A series of numbered characters are displayed – these represent the characters in a column
of text, and serve as a guide to set up the column widths, create as many columns as you
need, middle click to finish. Then set the row heights - one header row and one content row,
middle click to finish.

Hover over various positions around the table to select cells, columns, rows or the whole
table.

Select the table and enter its properties box. Define the text justification of the columns to
align in the centre of the cells.

Select the header cells individually and through the properties box [double click the cell or
right click > properties] add text to define the columns.
Create a simple repeat region for the information in the BOM and define the parameters to
display. This will means that the BOM table will be automatically expand downwards and be
updated as parts are added.

To define the cells included in the repeat region, either:

 If only some of the cells [as above] in the row are in the repeat region;
 Table tab > Repeat Region icon > Add
 pick the start and the end cells which define the extents of the repeat region
 annoyingly, there is no indicator that the region has been created
 Done and select a cell in the Repeat Region to highlight that region

or;

 If all the cells in the row are in the repeat region:

 Hover your cursor at the end of a row until it highlights
 Select the row
 Right click > Add Repeat Region

If the process gets confused - commonly having multiple repeat regions in one place - then
it is generally quicker to delete all the repeat regions and start again.

Table tab > Repeat Region icon > Remove > All Regions > Yes > select the table which
contain the regions

Assigned Report Symbols

Once the Repeat Region is created you need to assign the system parameters which will be
entered into the repeated cells. By using the Report Symbol option in the properties window
for the cells in the Repeat Region, the table can be automatically filled in.
  Double click the cell below No. and enter rpt. > index using the Report Symbol
option. This will number each part in the assembly.
 Double click the cell below Part Name and enter asm. > mbr. > name using the

Report Symbol option. This will fill in the part file name

 Double click the cell below Qty. and enter rpt. > qty. This will fill in the quantity of

each part

 To stop multiple instances of a part being displayed separately in the table: table tab

> repeat region > attributes > [select the Repeat Region] > no duplicates

Use the Update Table icon in the top toolbar to update the table to show the current part
information.

The Matl. column in the above example is empty at this stage as it was not included in the
repeat region. You could enter the material information manually via the cell properties.

Or you can assign a material to a part file [in the part file: Edit > Setup > Material] and then
using the Report Symbol asm.mbr.ptc_material.PTC_MATERIAL_NAME this can be
included in the repeat region. In the labs you will find the materials library in C:\PTC

Add BOM balloons to the drawing.

 Table tab > BOM Balloon > Set Region [select the Repeat Region] > Simple or
With Qty
 Create Balloon > Show > By View and then select the appropriate view of the
assembly where you want to place the balloon labels.

Reposition the balloons appropriately and change the attachment locations.

 Select a balloon and move it using the control handles

 Modify the attachment point of a balloon through RMB menu > Edit Attachment
 It is generally clearer if the attachment is to a surface rather than an edge

Make sure it is obvious what the balloon arrows are indicating

Nested Repeat Regions

If you have sub-assemblies in your assembly, these need to be included in your BOM. This is
achieved by creating a second 'nested' repeat region inside the initial repeat region.

The first table shows the definition points for the original repeat region. The second table
shows the pick points for the nested region. The following figure shows a table with a nested
repeat region. The regions do not overlap. If you mess up the Repeat Region allocation,
remove all regions and start again otherwise you are likely to get regions on regions.

When the table is updated you will initially have all components listed. You now need to
change the Attributes of each of the Repeat Regions to control the way the components are
listed.

Table > Repeat Region > Attributes

Hover over the table to highlight the top level or the nested repeat region. Select the required
Repeat Region and initially set both to;

Attributes > [select Repeat Region] > No Duplicates > Flat

Experiment with the setting Duplicates/No Duplicates/No Dup, Level and Flat/Recursive for
different listing combinations.
To remove extra cells (which are expecting sub asm components) under top level
components;

Attributes > [select nested Repeat Region] > Min Repeats > [set to 0]

Balloons

The convention is that as the sub assembly is listed as a component, you cannot create
balloons for the sub assembly items. Create a separate GA with table for the sub assembly
components.

Explode States

Showing an assembly in an exploded state can help visualise the components and how they
fit together. Always remember that you need to detail the assembled state - the explode
state alone does not ultimately show how the components fit together, sectioned views are
generally more informative.

To create an explode state which can be use in your GA you need to use the View

Manager in the assembly file.

See: Assemblies > Explode states & X sections

Then through the View Properties dialogue box (Dbl click a view) > View States > Explode
components in view. Through the Assembly explode state drop down list, select the
required explode state created in the View Manager.

Dimensioning Spline Curves

In its simplest terms a spline is a smooth curve with a constantly changing radius which
passes through a set of control points.

For further discussion look at this article [very accessible] or search on NURBS [Non-
Uniform Rational B-Spline] or B-Spline.

Because it has a constantly changing radius we cannot apply a complete dimensioning

scheme in our engineering drawing.
The first thing we need to define when considering how we might detail the spline is what is
its purpose in the design? If its a purely aesthetic feature which has no bearing or interface
with any other features then its details can be quite vague.

But if it interfaces with other elements then its definition must be more closely described. In
this case, in modern industrial situations, the electronic data will be referred to for any
manufacturing or modelling activities and a simple description would suffice in the drawing.

Remember that the the form of existing company logos are often very strictly controlled and
you would then only give its position and extents and a reference to the original artwork.

But situations will still arise where more precise detailing is required - the artefact is being
manufactured by manual methods, access to the original electronic data is restricted or
cannot be used by the manufacturer.

Datum point display style

To show a point of reference for the spline dimensions you will need to show the datum points
in the drawing - you would usually have these switched off. To control the graphical display of
the datum points:

Tools > Options > config.pro options

Option: display_point_tags Value: no

The above Option may have to be added to config.pro - in the Option box (btm
right) start typing the name of the option and the system will auto complete the
option, or use the Find facility. Add/Change the option to the list, save the
config.pro, copy it to your U:/ space if you want to use it for another session.

File > Properties > Drawing Options > bs8888.dtl options

Option: datum_point_shape Value: cross or dot
Option: datum_point_size Value: appropriate to line weight and sheet size

Method
Dimensioning each point is OK but can very quickly become cluttered - at least make sure
this is a detail view or a separate sheet.

A tidier method could be to put the X Y coordinates into a table - make sure you define and
dimension a point of reference.

To Save Spline Coordinates to a File

You can save spline points to a file with values in cartesian or polar
coordinate systems.
1. Select the spline you want to modify.
2. Click Edit ▶ Modify. The spline modification dashboard appears.
3. Click File. A dialog box appears.
4. Associate the spline to a local coordinate system.
5. Click the Save icon . The Save A Copy dialog box opens.
6. Enter a file name.
7. Click OK.

Creo creates a spline point definition file with the coordinate system
type printed in the file. The spline point definition file is a standard
text file that you can edit using the operating system editor.

Printing Engineering drawings

Printers:

A4 in XX001
A3/A4 in XX031
A0 at IT Services

Print dialogue window

To ensure the sheet print 1:1 - Print > Configure > Model > Full Plot

If there's an issue, you can centralise the border on the paper using the Offset options

Config options

To adjust line weight on laser printers - Tools > Options > pen[n]_line_weight

Pens 1 to 8 are assigned to different drawing entities

pen1 - solid edges - set to 2 as default but as long as you haven't got too much small detail
[lines will overlap] might be better set to 3

pen2 - dimensions

WYSIWYG - what you see is what you get.

Turn off reference geometry - planes, axis, csys, points.

Hide datum curves - use your layers

Printing to PDF

The Save as PDF option directly from ProE is not brilliant - it may show hidden line and axis
as solid dependent on the scale of your view - something to do with working in metric units!

In XX001/2 > File > Print and choose the PDF generator in the printer list - this will give you a
better PDF. You may have to tinker with the Pen Weight options as mentioned above

3D Data Standards

With the increased dominance of CAD systems in the design and manufacture process there
has been an increased need to standardise the use of the core 3D data rather than 2D
drawing for documenting a form.

Here are the two relevant standards:

ISO:16792 - Link

ASME Y14.41-2003 - Link

CNC Machining in the Department

A majority of high volume consumer products still have a heavy reliance on injection moulding
to produce the component parts. CNC machining in the Department will give you an insight
into the issues - capabilities and restrictions - of the process and help you design products
which will need fewer changes in the downstream design process and will therefore get to
market quicker.

These pages guide to you through the procedure required to produce a file to drive the CNC
milling and routing machines in the Department.

This section is primarily aimed at students undertaking the Design for Manufacture
Injection Mould Tool project but is equally applicable to any CNC machining.

If you would like to use these machines outside of the usual modules then please talk to SPK
regarding your requirements.
CNC vs RP discussion here

Our machines, their application and capacity.......

Denford Milling
Machines - 3 Axis

Boxford Router - 3 Axis

Unimatic Router - 4 Axis

Cybaman Replicator
5/6 Axis

Denford Lathe

DP4 Machining Considerations

Because of time limitations in the DMT module, we have restricted
machining geometry to 2½D Machining.

2½D Machining refers to the action of removing material in z slices with the tool moving
through 2D x,y coordinates. Therefore the tool feeds vertically down into the material to a
specified depth and the then moves horizontally around that x,y plane removing material, it
then feeds to the next z increment vertically down and removing another layer of material.

Machining complex 3D surfaces or non horizontal planar surfaces to an adequate surface

finish requires a very small stepover [to minimise scallop height] with a ball nosed cutter - this
will result in a long machining cycle, maybe 2 or 3 hours for a relatively small surface. There
are also more complex considerations for merging into neighbouring surfaces which can take
a lot of time to solve.

Above: scallops produced with ball nosed cutter on 3D surface

So, as you are considering your design and procedure sheet remember that the main
restrictions are that you cannot machine any sloped or curved 3D surfaces and that you are
limited in the shape and size of tools available. This is particularly important when considering
z depths – a good ‘rule of thumb’ is that a tool may start to flex if it is greater than 1½ times its
diameter in length.

Split your tool into elements

To complete your procedure sheet you need to consider how each element of your mould can
be best machined in terms of the tool type and size and the path it will take when removing
material.
It doesn’t matter what geometry you’ve constructed in your reference model, the tool
type and size and the path it takes will ultimately decide how the cavity will look.

Example: The reference model above left contains a rectangular cavity. If this was finish
machined with a ball nosed cutter the result would be the cavity in the block on the right – you
cannot machine the vertical square corners with a cutter in the standard orientation on the z
axis.

There are two further issues with the resulting cavity (diagram above);

• firstly, it would have to be machined in two stages as the flat area in the bottom could not
be produced with the balled nosed cutter – this would leave grooves [scallops] across the
bottom of the cavity. A cavity which is smaller in x and y by the corner radius all round would
have to be machined with a flat bottomed cutter.

• secondly, if we consider the previous image, there would be a small amount of material
where the cutter used for the inner cavity would not be able to blend completely with the
surface produced by the ball nosed cutter used to machine the perimeter. This material can
be removed with some careful consideration.
Preparation

*** Good file management is absolutely critical at all stages of the

project, a lot of associated file will be created automatically which
need to be kept together in a separate project folder ***

Reference Model

You should have a part file of your tool – this is your Reference Model - what you going to
create. We use the geometry in this model to guide the tool path - edges, curves, surfaces,
volumes, holes, etc. - this is dependent on which mill geometry or sequence type you are
generating. It may not be an exact image and may have to be adapted to produce the
desired geometry.

Workpiece - the stock material

When you open a manufacturing file a default Workpiece is automatically assembled.

Important concept: The Workpiece defines the extents of the stock material (as this could
be larger than the reference model) and therefore where the machine will create tool
movement data.

You will need to resize the default Workpiece to represent your stock material.
Open a new Manufacturing file

Default files

The above screenshot of the model tree in a new Manufacturing file shows that there are a
number of files automatically created and assembled - it is important these files stay
together in your project folder.

You will not find unique manufacturing file in the working directory. All the
manufacturing info is saved in the Assembly file
The four part files represent the physical setup of the machine prior to machining. The last
three files allow you to visualise any tool collision issues - they do not influence the machining
process. The Group MC_SETUP can be hidden once considered - save your layer status to
keep items hidden when a file is reopened.
 Assemble Reference Model
Next assemble your reference model in the correct position relative to the Workpiece.

Use the Assemble Reference Model icon in the right toolbar

DO NOT use Insert > Component > Assemble

DO NOT drag and drop your reference model into the assembly

File Management

1. [project].asm - assembles your workpiece, clamps and reference model

2. mc_workpiece.prt - the default workpiece - 150 x 100 x 25mm
3. mc_bed.prt - the machine bed
4. mc_set_strip.prt - xy the datum setting strip
5. mc_clamp.prt - the workpiece clamp
6. [reference model].prt - reference model
By this stage you have six files which are critical to your manufacturing file reopening
correctly.
Once you have finished your first session with your manufacturing files, it is critical that you
move all these file to a project folder.

When you return to your project:

- move the folder to the Working Directory

- RMB on the folder in Creo and set it as your working directory

- when finished, move the folder off the hard drive and overwrite the existing folder

Interface

1. Volume Roughing
2. Previous Step - Local Milling - 'rest mill'
3. Trajectory Mill
4. Standard Drilling
5. Engraving
6. Surface Mill
7. Sequence Parameters
 8. Cutter Path Simulation
9. Process Manager
10. Tool Library
11. Insert Workpiece
12. Create Mill Window
13. Create Mill Surface
14. Create Mill Volume

Tooling

* See the Parameters section for tool spindle speeds and feedrates

You will need to ensure that all the tools you need – these will be in your CNC procedure
sheet - are setup within the machine setup. You can enter the tooling setup through Menu
manager > Mfg Setup > Tooling. Or whilst editing the sequence - setup > tool

Setup the:

number - in setting - do not repeat

name - give it a logical name

type - ball mill, end mill, drill, etc.

 geometry - dia., length and ball radius if applicable

and then apply to the tool list.

Make sure each tool has a distinct number [not name] as this is the only information
which is transferred to the final CNC file

Ensure that all tools feed more slowly vertically into materials than horizontally through
material - parameters > advanced > horizontal feed

Slot drill - Flat bottomed cutter which can feed vertically down into material. Vertical feedrate
needs to be less than horizontal feedrate

Ballnosed cutter - the corner radius of the tool is equal to the major tool radius. Can feed
vertically down into material. Vertical feedrate needs to be less than horizontal feedrate

Drill - standard 118 degree point helical fluted drill

Engraving tool - a simple 'burr' tool with a pointed end. The main body of the tool is 6mm
diameter and will therefore need 3mm clearance around the tool path.

Mill Geometry

Definition: Geometry which limits the tool movements

Major use: Mill window - curve [sketch or edges] which defines x y boundary. Tool
machines stock material inside boundary until it encounters reference model surfaces.
Mill Window

Video Here

Method:

 Select a Window Plane (sketchplane)

 In the Dashboard, select the Sketch window type icon
 Select the front (not top) face of the block to face downward
 Select sketch references
 Sketch or copy edges to create window
Under Options the default is to limit your tool movement to inside the window, this can be
changed to on or outside the window.

Mill Volume

Select surfaces or create a feature to represent a Mill Volume. Selecting surfaces is a long
process, it is usually easier to use extrudes etc. or use a Mill Window.

You can create rounds on your Mill Volume. Once you have the volume feature completed,
click on the Mill Volume Tool icon in the right toolbar and select the Round tool icon in the
right toolbar. Select the edges in your mill volume.

Referencing existing edges

An underused tool which is essential when creating Mill Windows is the Use [copy] Edge
tool in sketcher. A mill window needs to be robustly referenced to the edges in the reference
model - if your reference model changes, the mill geometry will change.

The cutter may also follow a curve in a Trajectory sequence, in this case the curve is
selected within the sequence.
Setting up a machining process

Before you start any sequence make sure you understand what you are proposing in practical
terms, visualise going through the motions in a practical session in the machine shop. This
will tell you all the information needed to make the sequence successful.

We shall primarily be using:

 Volume Roughing [by window]

 Previous Step - Local ['rest'] Mill

 Trajectory Milling

 Engraving

 Holemaking

You can also use surface milling but this will not be supported in the Des. Manuf. module -
see the 3D Machining section.

As you build the NC sequence you assign three main elements:

1. Tool

2. Parameters

3. Geometry

All of these elements can be redefined.

To start a Sequence

Choose the appropriate icon in the top toolbar.

You need to ensure that at least Tool and Parameters are ticked in the SEQ
SETUP menu.
The geometry will be specified by different methods dependent of which
sequence type you are constructing, ie. for an initial Volume Roughing you
should choose Window in the SEQ SETUP menu to define the geometry to be
machined.

To Modify a Sequence
Simply RMB > Edit Definition in the model tree as you would a model feature.
Tick the element you wish to modify and click Done

Tools
See the Tooling section for setting up a tool for your sequence

Parameters

We are looking for the most efficient sequence types, sequence order and setting within the
sequence which will minimise the machining time and maximise surface quality.
The figures and options set in the Parameters Window control how the machine executes
the chosen sequence – spindle speed, cutter feed rate, step depth, the order that elements
are machined, etc. Options highlighted yellow are minimum requirements for the sequence
to function.

Ensure that all tools feed more slowly vertically [plunge] into materials than
horizontally through material.

These Parameters will have to be ‘fine tuned’ to achieve the desired effect within the
machining sequence. The Parameters Window can only be entered whilst setting up or
modifying a sequence and the parameters are particular to that sequence.
It has two levels – Basic and All – showing more or less parameters. You can also view

parameters by category. Use the Manufacturing Parameters Tree icon in the top

toolbar to enter the parameters window whilst building a sequence.

Geometry
All sequences need to know where in the cavity geometry it is going to be
applied. This definition will be different according to the sequence type, ie. a
hole will simple need a coordinate (defined by an axis, point or cylindrical
surface) but a trajectory mill will need a chain of edges or curves.
Geometry selection will be dealt with within each sequence description.

Volume Roughing

Video Here

This sequence will remove a volume of material defined by the reference model. A Mill
Window is the simplest method for defining the part of the reference model to be machined.

From the SEQ SETUP menu, ensure the minimum setup requirements are checked;

 tool
 parameters
 window

Click Done.

Select or set up the cutting tool, click OK.

Set the required parameters through the parameters window – this window has a Basic (the
basic parameters) or All (all parameters) condition. (specialised parameters are discussed at
the end of this section).

The next step is to select the window - see Mill Geometry section.

Once you have selected the window you will be returned to the NC Sequence menu.

Choose Play Path to simulate the sequence.

Choose Seq Setup to redefine any elements of the sequence.

** The Sequence is not complete until you select Done Seq **

Parameters

In the parameters windows, you must set:

CUT_FEED

PLUNGE_FEED

STEP_DEPTH

STEP_OVER

CLEAR_DIST

SPINDLE_SPEED

Other preferred options for a volume mill are:

SCAN_TYPE FOLLOW_HARDWALLS

ROUGH_OPTION ROUGH_ONLY

RETRACT_OPTION SMART

ROUGH_OPTION settings

Controls whether a profiling pass occurs during a Volume milling NC sequence, this will
machine the perimeter of the volume. The options are:

ROUGH_ONLY Creates an NC sequence with no profiling.

ROUGH_&_PROF Creates an NC sequence that rough cuts the milling volume, then profiles
the volume perimeter.
PROF_ONLY Only profiling is done.

Using PROF_ONLY could allow us to avoid a trajectory mill sequence if we use it in a new
sequence with a different tool to finish the perimeter of a previously machined volume.

SCAN_TYPE settings
Controls how the tool moves in the cavity at each slice depth and how it deals with islands or
holes in the cavity. The options are:

TYPE_1 The tool continuously machines the volume, retracts upon encountering islands.
TYPE_2 The tool continuously machines the volume without retract, moving around the
islands upon encountering them.
TYPE_3 The tool removes material from continuous zones defined by the island geometry,
machining them in turn and moving around the islands. Upon completing one zone, the tool
may retract to mill the remaining zones.
FOLLOW_HARDWALLS The tool will follow a path which is approximately concentric with the
perimeter of the cavity.

TYPE_3 and FOLLOW_HARDWALLS are generally the most efficient options for this
sequence.

You will have to experiment with different parameter combinations and selection options to
obtain your desired effect – remember it is very easy to redefine the sequence through the
menu manager or through the parameters window (see Modification of NC Sequences on
page 6).

Helical Approach

Unlike a Slot Drill, a 4 fluted cutter cannot plunge vertically into a volume to a slice depth as it
does not have a cutting edge across its axis. A Helical motion means it is cutting on its side
as it plunges.

Parameters
RAMP_ANGLE [try approx 5 deg]

HELICAL_DIAMETER

Previous Step - Local Mill

This sequence will refer to a previous sequence and, using a smaller tool, calculate if there
are is any more material which can be removed.

With Select highlighted in the SELECT FEAT menu, choose select the required
sequence in the model tree.

Select the CUT MTN

Check Tool and Parameters

Choose a (smaller) tool which will get into all the nooks and crannies left by the previous tool

Trajectory Milling

* If your machining complex line work such as a logo then use the Engraving sequence

Video Here

Trajectory Milling will follow a defined path which is selected from edges or curves within
your reference model. The shape of the tool, its position relative to the trajectory and
z depth relative to the machine zero define the cavity formed.

Important - It is unlikely your cutter can take out all the material in one pass, make sure you
consider the settings below to slice the total depth. Ball nose cutters in particular will need
more than one pass to give a good surface finish

Start a Sequence

Choose the Trajectory Mill icon from the top toolbar

Choose 3 Axis > Done

Check Tool, Parameters and Tool Motions

Setup the Tool.

Set up the usual Parameters.

OK will take you to the Tool Motions window. Choose Insert to enter the Curve Trajectory
Setup window.

Select the curves or edges which define the trajectory - remember to use the chain
selection method [shift]

DO NOT [generally] specify a Start Height

The Height parameter specifies the total depth of cut – pick a surface or datum plane.

Through Tool Offset set the tool to run on the trajectory [None] or offset by the radius to the
left or right.

OK to return to the tool motions window

Redefining the trajectory

Choose the Curve Cut element in the Tool Motions window, right click, Edit Definition to
return to the Curve Trajectory Setup window

To add further chains to the same sequence

Don't create separate sequences for a group of trajectories which have the same cutter, depth
and parameters.

Select <end of tool path> in the Tool Motions window

Select Insert again to return to the Curve Trajectory Setup window - repeat above

Slicing the Total Depth

DO NOT remove the material in a single cut - you need to slice the total depth into slices -
see above image.

Set up the parameters STEP_DEPTH and NUMBER_CUTS [number of cuts] - this slices the
total depth from the bottom up. Once the tool path is running you may have to fine tune
these values. Choose All rather than Basic in the displayed list of Parameters.

Zig Zag
Rather than returning to the start of the trajectory for each slice, set the parameter CUT TYPE
to ZIG ZAG - this will force the cutter to cut in both directions. Choose All rather than Basic
in the displayed list of Parameters.

Remember the Manufacturing parameter tree icon in the top toolbar when fine tuning the

sequence.

Standard Drilling

DO NOT drill any holes deeper than 10mm - there is a likelihood that the drill
flutes will become clogged and the drill break. If your hole needs to be deeper
than 10mm deep, then drill a 10mm pilot hole which can be completed in the
machine shop.

Sequence setup

Select the Standard Drilling icon from the top toolbar

The default setting is to select axis or cylindrical surfaces to define hole

positions, this becomes the Hole Set

Next set the hole depth by specifying the start and end.

DO NOT use the the default Auto setting as this is likely to drill through the workpiece. Ensure
that any depths are Blind (to a defined depth) and are set relative to the start surface of the
hole set and the Tip of the drill

DO NOT drill through the stock material.

DO NOT use a negative figure for the hole depth – drill can only drill downwards so the
direction does not need to be defined and you do not have to specify the depth as a Z
coordinate.

.
Hole drilling order

Under the Options tab you can choose which hole is to be drilled first. The order of
machining the holes can also be influenced by the SCAN_TYPE parameter value.

Engraving

For machining complex line work at a single depth such as a logo. See Level 2 Modelling >
Geometry from 2D graphics for some info on exploiting logo images.

Define the engraving tool as 0.5mm diameter and machine to 0.2mm depth. The shank of
the tool is 5.0mm - watch for collisions with side walls in cavities - see below
In your Reference Model part file generate a Groove [cosmetic] feature

 Insert > Cosmetic > Groove. [This function is in the old 'Menu Manager' style]

 Choose the surface you want to project the feature onto

 Choose the sketch plane
 Choose a plane to orient the sketchplane
 Sketch the curves

Pick the Engraving from the top toolbar

  Tool
 Parameters > set the usual parameters, do not set NUMBER_CUTS
 Parameters > make sure you set a GROOVE DEPTH
 Groove feature

Process Manager

Once you have a number of sequences in your model tree it can be quicker to
navigate, simulate and modify your sequences through the Process Manager -
top toolbar.

The default columns are not particularly useful for our purposes. Copy the configuration file
step_table_setup.clm from the default working directory (c:\user_files\ptc) into your
working directory (your project folder) to change the columns.

In the first column pick the operation name or a sequence name and use the right
click menu for various options. Use the bottom toolbar to edit or play the selected
sequence.
Tool Movement Simulation

Before simulating toolpaths;

 Unhide the workpiece

 Hide the Group MC_SETUP - machine parts
 Switch to wireframe

You can use the RMB > Play Path option in the Model Tree to play individual
sequences or the whole Operation.
The Play Path option is also available whilst editing a sequence and in this mode
gives you access to NC Check

Sequences can also be played via the Process Manager.

Simulation

Once your sequence has been created you can simulate the tool movement in two ways:

Cutter Line motion (CL Data)

This is the default simulation method and the clearest for considering tool movements. The
motion of the tool will be simulated and 3D lines will be created joining the coordinate points
calculated within the sequence. You can tumble the model whilst the tool is moving.

NC Check

This is a ‘virtual machining’ process in which the Workpiece is shaded and material is
removed as the tool movement is simulated. NC Check is not available via the RMB menu.

NC Check image quality

Changing to a 1x1 Resolution with give a higher resolution motion

display if you are after more detail or a screen dump.

NC CHECK > Resolution > 1x1 pix

Post Processing

Once you have completed all the sequences required for your machining process they need
to be interpreted into NC machine code for the specific machine you intend using, this
process is referred to as Post Processing.

The process will generate a simple text file with the extension .tap which you will find in the
working directory. The .tap extension may have to be changed according the machine you
are going to use.

Through the drop down menus:

Edit > CL Data > Output

Operation> [select your operation name]

File> [tick the MCD File checkbox] >Done

An .ncl file needs to be generated, give it an appropriate name say, your user ID – this will be
the name of your .tap file - and click Done

Leave the defaults in the PP OPTIONS menu and click Done

The PP LIST then offers you a number of Post Processor files;

UNCX01.P01 Denford Mill

UNCX01.P02 Denford Mill - no arcs

UNCX01.P03 Denford Mill - Easimill/Heidenhain

UNCX01.P04 Denford Router - no arcs

UNCX01.P05 Denford Router - with arcs

UNCX01.P06 Boxford A3HSR Router

UNCX01.P07 Boxford 500HSR Router

This file can be viewed with a standard text editor. Some outputs will require a small amount
of manual editing before submitting to the machine. The file consists of x,y,z tool movement
coordinates, and control codes.
M codes are machine control codes;

M06 is a tool change, followed by the tool number T.

M03 starts the spindle at the appropriate spindle speed S.

M05 stops the spindle.

G codes are movement control codes;

G0 is a rapid positioning movement whilst not cutting.

G1 is a linear movement at a feed rate F.

G2 and G3 are clockwise and counter clockwise arc movements.

G80, 81 and 83 are drilling cycle codes.

Right click, 'save target as' or click for print friendly version

CNC Procedure Sheet

Grp: Job:

Tool
Sequen
Numb
Tool Too Sequen
ce Diamet
Number er * er l ce
 Typ Descrip
e tion

* If the same tool (type and diameter) is used in different sequences it retains the same
tool number.

CNC Machining Tool Parameters

Parameters for Slot Drills on aluminium

Horizontal Maximum
Spindle Plunge Step
Tool Dia. feed rate [total] depth
speed feed rate depth
[cut_feed] of cut
2.5 6000 100 60 1 2.5
3 6000 200 60 1 6
6 5000 250 60 1 12
8 4000 300 60 1 14
10 3000 300 60 1 16

5.8 drill 2500 - 60 - 10

0.5mm 6000 200 100 0.2 0.2

Engravin
g
 Tool

Remember to set a plunge feed rate – found in the Advanced area of the parameter
window – all tools must feed more slowly into materials than horizontally through
material.

Diameters between those stated are also available in 1mm increments.

All feed rates are in mm per minute.

Ball Nosed cutters - decrease feedrates by 20%

Tools above 10mm dia. can be used but are restricted by machine power and the clamping
system used - seek appropriate advice.

Maximum Depth of Cut

Whether it's a slot drill or ball nosed cutter, our standard tool range has either a
6mm or 10mm shank diameter. The cutter diameter will be equal to or less than this
dimension - see below image. The maximum depth of cut is restricted by the length of the
cutting edge, therefore if you want a 1.5mm radius in the corner of a pocket, that pocket can
be no greater than 6mm deep – the cutting edge length of a 3mm dia. tool.
Engraving Tool
This tool will produce a line on a surface 0.5mm wide with a depth of cut of
0.2mm. This will show as a raised line on your widget and can be used for
lettering and logos. Use with a Trajectory Mill sequence. Watch out for
clearance from side walls in cavities - see below.
Tool Spindle Speeds and Feedrates

Surface Speed

A particular cutting tool material has an optimum speed at which it

should travel through a particular material.

Example: The tip of a High Speed Steel [HSS] cutting tool should
travel through aluminium at 150m/min.
Therefore we need to control the tip speed of the milling cutter at the radius of the tool - its
circumference [in metres] multiplied by its revolutions per minute.

Spindle Speed

Spindle Speed = Surface Speed / Circumference

For a 10mm [0.01m] dia. cutter:

circum. = Pi x Dia = 3.14 x 0.01 = .0314m

For a cutting speed of 150m/min: 150m/.0314m = 4777rpm

Free cutting mild steel 38 m/min

Low carbon steel 32 m/min

Brass or bronze 55 m/min

Aluminium Alloys 150 m/min

Plastics 250 m/min

Woods 500 m/min

Feedrate

Feed rate is the distance a cutting tool moves through the

material per minute.

This rate dictates how much material each tooth of the cutting tool removes per
revolution.

Feedrate is dependent on the:

 Surface finish desired

 Power available at the spindle (to prevent stalling of the cutter or workpiece)
 Rigidity of the machine and tooling setup (ability to withstand vibration or chatter)
 Strength of the workpiece (high feed rates will collapse thin wall tubing)
 Characteristics of the material being cut, chip flow depends on material type and feed
rate
 The ideal chip shape is small and breaks free early, carrying heat away from the tool
and work.

Feed rate (mm/min) = Tooth Load (mm). X Number of teeth. X Spindle Speed in
RPM.
Denford: http://www.denford.com/Feeds and Speeds.html

Wiki: http://en.wikipedia.org/wiki/Cutting_speed

3d Machining

In this section we will consider strategies and setting for machining complex 3D or non
horizontal [XYplane] surfaces using the 3 axis CNC machines. Two fundamental issues to
understand and overcome are surface finish and the minimum curvature on the machined
surfaces.

Surface finish - Scallop height and ballnose cutters

Surface accuracy - Smoothness or Roughness

We cannot use a flat bottomed cutter to machine a non planer surface, therefore all your
machining must be done with ballnosed cutters. A ballnosed cutter will machine its profile
through the material producing a groove across the surface which has a radius equal to that
of the cutter.

Therefore the combination of the cutter diameter and the stepover will dictate the surface
finish. In the image above both the 20mm and the 4mm ballnose cutters are machining with a
1mm stepover. The smaller diameter will produce the coarser finish - using the largest
available cutter will give allow the best surface finish and shortest cycle time. [Surface finish
discussion here]

The deviation from the original surface [being followed by the tool tip] and the highest point of
the groove is referred to as the cusp or scallop height.

The other important factor which controls the deviation from the reference
surface is the number of coordinates output for toolpath.

Radii or Spline

CNC controllers will move two axis simultaneously to produce a planar radii. The
code will specify the start and the end coordinates and the radius (R) or arc centre
(I and J).
Controllers cannot follow a spline exactly as it has a constantly changing radius.
Instead the spline is split into facets, the software outputs XYZ points along the
spline. The number of points the spline is broken into is defined by accuracy
setting in the CNC software which defines the chordal deviation from the
reference surface. It is also defined by the curvature of the spline - a higher
curvature will require more points to achieve the same chordal deviation.

1. Chord deviation 2. Reference surface 3. Chord

Click above image to enlarge

Cutter choice

The ballnose diameter we choose for as particular sequence is dictated by many things -
availability, machine power, spindle capacity.

The most important factor is the minimum radius in the area you wish to machine

Suggested strategies and sequences

Volume mill by Window with 20mm flat bottomed

Surface Mill by Window initially with 20mm ball nosed cutter

Isolate smaller areas by window with smaller ball nosed cutters

Unimatic Router - 4 Axis

Movement: X 1000mm Y 1200mm Z 240mm Linear

Max material size is dependent on cutter dimension with the above axis travel limits.

** Your material height [including base board] must not exceed 120mm
**

Rotary 4th axis capacity: 160mm dia. x 600mm length

Max feedrate: 4m/min

Roughing Cutter

20mm dia. flat bottomed

1500mm/min horizontal feed
500mm/min plunge feed
10,000 rpm spindle speed
5mm step depth

Finishing cutters - ball nose

3000mm/min horizontal feed

500mm/min plunge feed
16,000 rpm spindle speed
Distance X dictates the maximum depth of cut - approx 110mm

Distance Y has to accommodate the fixing plinth for the job, the thickness of the workpiece
and the tool clearance height.

Tool Clearance
To get maximum depth of cut we can use long series cutters or an extension arbor as
pictured above.

Which ever method we use, the 25mm dia. clamping nut will need to be considered for side
wall clearance when using cutters less than 25mm dia.

Material Clamping

Consider clamping setup *here*

Minimum 10mm thick MDF for base board.

7mm dia. holes drilled at suitable centres in 50mm increments.

Make sure there is adequate cutter clearance around workpiece to baseboard securing
screws.
* IMPORTANT * - make the wood screws you use to secure the workpiece onto the base
board do not protrude into areas which will be machined - this will scrap the router cutter.

SK20 Collet

ProE Plastic Advisor

Plastic Properties

Name: Exxon LDPE Escorene LD 605 BA

Suggested Melt Temp: 200 degC
Suggested Mould Temp: 30 degC
Melt Index: 6.5 g/10min
Density: 0.924 g/cm3

From ProE:

Open your Widget file, NOT your mould tool

Application > Plastic Advisor - DO NOT select an injection point

First pick the Injection Point Location.

Then go to the Analysis Wizard, select Plastic Filling and pick Next.

*The LDPE used in the Department, as detailed above, is not included in the database in
Plastic Advisor. To set up this polymer you will have to find a similar product, Copy its
properties and then Edit its characteristics.

Once you have chosen an injection location, select the next icon along the toolbar – the
Analyze button. Once the analysis has run you can consider the report from the system and
view different types of results using the Result Type drop down selection window on the left.

You can also consider weld lines (where two ‘fronts’ of flowing plastic come together) and
look for air traps.
 Simulation
** Warning - asm. referencing

A 'Top Down' design approach using references from other parts within the asm. can cause
failures if you then start moving those parts relative to each other using connections - pretty
logical really. Use Copy Geometry rather than picking up the refs directly.

Mechanisms

The mechanism extension allows you to simulate and analyse a mechanism which has sliding
and rotating joints. Once the assembly has been created it can be simply dragged on screen
or motors can be attached to the joints which will simulate a controlled movement through an
analysis.

We have both the Kinematic [simple movement] and Dynamic [movement influenced by
gravity and friction] license. The Dynamic module is not taught in the Department.

Animation

The Animation extension is primarily a presentation tool which outputs an Mpeg video file.
In its simplest form we could look at a model from different camera angles or we could
explode and reassemble the model, view from different angle and have motors driving our
joints.

Manually Positioning Parts - 'dragging'

Whether in standard assembly mode, mechanism mode or animation mode you will need to
move parts within their degrees of freedom.
Use the Drag icon in the top toolbar to enter the Drag dialogue box

Dragging can become problematic when you are at the end of a chain of connected parts with
various degrees of freedom - try dragging the end part and all the other parts follow. Imagine
trying to position a finger relative to a hand and the hand and arm moves out of position as
you drag.

There are various temporary constraints in this dialogue box which are useful when trying to
accurately position a part.

 The Body-Body lock constraint allows you to lock the parents of the part you are
positioning so only the one part moves.
 Select a part as the static 'ground' part [or MMB/OK to use the environment]
 Select the part or parts in the 'chain' which you don't want to move. MMB or OK to
finish.
 Now if you drag the next part in the chain, it will move independently.

Mechanisms
Before you proceed with the mechanism extension you need to fully understand assemblies
and Degrees of Freedom (DoF). Be careful with your reference selection - generally only
choose references from two parts to make a connection.

The mechanism extension allows you to simulate and analyse a mechanism which has sliding
and rotating joints. Once the assembly has been created it can be simply dragged on screen
or motors can be attached to the joints which will simulate a controlled movement through an
analysis.

Joints can be limited in their range of movement and a motors characteristics need to be
carefully considered. An analysis can then show any interference between parts, trace a
curve of the mechanism motion or create a movement envelope.

Some steps are carried out in the standard Assembly environment, some in the
Mechanism extension - Assembly > Application > Mechanism

The fundamentals steps are:

 Assemble and connect/constrain base part as ground

 Assemble moving parts with Connections, fixed parts with Constraints

 Set connections limits where needed

 Move into the Mechanism extension

 Create Mechanism specific connections - gears etc.

 Apply and setup Servo Motors to driven Connections

 Set up Analysis

 Run Analysis

 If required - Replay Analysis checking for interference

Tips

 If you want the base part to move out of the scene, connect it to the assembly csys
using the weld connection – this can then be disconnected
 Be careful how you connect subassemblies – ie. if you have an arm pivoting on a
body and then an entity constrained/connected to that arm - if that entity is related to
anything other than the arm it may not allow the arm to move

 Always consider your Limit Settings

  When defining/editing a Motion Analysis consider how the initial configuration
(through the analysis or motor settings) of an entity is controlled – this will stop parts
flipping to an inappropriate configuration when the analysis starts

 Create a ‘start position’ Snapshot

Common Connections and use:

Weld - aligns two coordinate systems - allows disconnection for animation

Slider – one axis/edge sliding along another axis/edge with no rotation around the axis/edge.

Pin – axis/edges aligned allowing rotation around the axis/edge but no translation along it.

Cylinder – either - to allow rotation and translation on an axis – rotational and slider motors
can be attached to the connection – or – in combination with a separate but parallel pin
connection to avoid conflicts.

Limits

Most connections have the facility to limit the movement of a joint and set a zero and
regeneration position. You will need to specify a zero reference on each of the parts to
enable this function.
Servo Motor Profile

For constant motion in a single direction choose make the Specification velocity and the
Magnitude constant.

For a reciprocating motion make the Specification position and the Magnitude cosine.
Consider the Graph to determine the effect of variables A, B, C and T. Use the Initial Position
preview to determine where your zero point is.

A = amplitude – the distance the motor will reciprocate through

T = period – time through a full cycle

B = phase – degrees - offsets the cycle along the time line

C = offset – mm - offsets the cycle along the amplitude line

Animation

The Animation extension is primarily a presentation tool which outputs an Mpeg video file.
In its simplest form we could look at a model from different camera angles or we could
explode and reassemble the model, view from different angle and have motors driving our
joints.

Over a set time period the system creates frames (x images per second) which represent a
smooth transition from one ‘camera’ position to the next and, simultaneously, from one
assembly state to the next. Motors may also be driving joints whilst the scene changes.

Creating a good animation relies on your creative skills not your CAD skills. Good planning
and a good storyboard with plenty of fine tuning will make a good presentation video.

'Tweening'

Although a standard video is made up of 25 frames (images) per second you do

not have to create each of those frames. You create Key (significant) frames
and the system generates the frames between these frames.

The transition tweening process starts immediately after a key frame so if you
want to hold a View (camera position) or Transparency you will need to have
two instances of it in the timeline separated by the required hold time.

Do not have your assembly bouncing around the screen when your meant to be showing
the mechanism characteristics.
Snapshots

A saved assembly state with or without connections disabled. You cannot disable a
constraint, so if you want to disassemble non moving parts you will have to use Rigid or
Weld connections which can then be disabled.

View

A camera position. Create these with the top toolbar Named View List icon in the part file.
Don't confuse Snapshots with Views.

Fundamental steps (these assume you are starting with your mechanism assembly):

1. Plan Animation on paper - views/zooms/explodes/timeline/motors

2. Enter Animation module

3. Create snapshots as you disable joints and explode the assembly

4. Create views/zooms

5. Right click seconds ‘ruler’ to edit Time Domain

 6. Create new Key Frame Sequence - KFS - add snapshots at appropriate time

intervals

7. Add views – use the View @ Time icon

8. Add existing Servo Motors – Animation > Servo Motors – motors cannot be

active if their joint is disassembled.

9. Run the Animation – use the black circular Start Animation icon

10. Adjust the elements and Run the Animation again to update it

11. Playback the Animation – use the triangular Playback icon

12. Use the Capture button to export the Animation

Snapshots

Animation module > Drag Components > Snapshots

Drag components to required position > create Snapshot

You then have a collection of assembly states in your list which can
be included in the KeyFrame Sequence. They can be used in any
order and multiple times.

To allow you to 'explode' an assembly;

Constraints tab > Enable/Disable Connections > select the

Connection to disable

Now that components can be drag apart from the assembly. The
dragging will be very imprecise unless you use the Advanced Drag
Options to control the direction of the component.
To add new Snapshots to an existing Keyframe Sequence;

Select the KFS > RMB Edit KFS > add Snapshot at time

Conflicts

Keyframes - don't have multiple Keyframe Sequences on one

timeline as the assembly states will conflict.

Motors - motors cannot run if their parent parts are disconnected or

if another motor is running a conflicting motion.

Transparencies

Consider the Tweening advice above, you will need to set an initial
opaque transparency before your clear transparency. The time
between the two decides how quickly the selected part becomes
tranparent.

In the example above the part remains opaque till 5s then turns transparent by
6s, is held transparent till 9.5s then returns to opaque by 14s.

Display @ Time

Another method for showing hidden or internal detail is to use Style

states from the part model. Use the View Manager to set parts in
different display states eg. leave the internal parts Shaded and the
external covers in Wireframe. Style states toggle on/off instantly
so you do not need the method as described above for
Transparencies to manage transitions.
Tips

 Create animation snapshots as you gradually explode an assembly rather then fully
exploding an assembly and then bringing it back together

 A view does not contain any information about the position of the parts but simply a
distance and position for viewing the scene – the parts may in any state of assembly

 Equally, Snapshots do not contain any view information, it is simply a relative

position of all the parts.

 Consider whether you can have a particular snapshot and motor in the same place on
the timeline - you cannot have a particular assembly state [snapshot] and motor
controlling the position at the same time.

 Do not have your assembly bouncing around the screen when your meant to be
showing the mechanism characteristics. Repeat a view in the timeline to freeze the
camera position before moving the next view.

 Make sure the frame rate in your timeline [RMB the timeline > edit time domain] is
aligned with the capture frame rate when your ready to output the .mpeg file. By
default these will be different.

 Remember the .mpg output is a screen dump. Turn of the reference geometry and
spin centre, hide datum curves and increase the display quality - View > Display
Settings > Model Display. Put some colour in your model and change the light
setup.

Introduction to 3D rendering.

3D rendering software creates an impression of your CAD model as if it existed in reality. An

image which gives an impression of surface textures, surface colours, shadows, reflections
and highlights at a basic level and then more advanced environmental effects such as depth
of field, light scatter, camera lens flare, fog effects.

Physical properties are created on the model and then an environment is created around the
model.

As you progress through the rendering process remember that many of the effects you
create, such as surface appearances and lighting setups can generally be saved separately
from the model and used with other models. In this way you can start to build up your own
library of render resources.

3D rendering in ProEngineer

Although Creo cannot produce very high quality render outputs, there are some distinct
advantages to using it for 'quick and dirty' renders:

 full associativity to the model

 avoidance of data translation issues
 render setups can be saved in the model and be saved to use on other
models

By default, rendered images in Creo [.prt or .asm] will use the

module ARX (Advanced Render Extension). You will see this
referred to as Photolux in the ProE environment and is based on
the Mental Ray render engine.

Render Toolbar

All the functions needed to set a scene and to render it can be accessed from the Render
Control menu bar.

If it's not showing, RMB on any active icon in the top toolbar and display the Render toolbar

To create a scene, you need to consider these sections:

Keeping it simple and experimentation are the keywords for rendered output
from Creo.

Help > Manual for the full instructions

File format: .bip – the model, scene and materials are saved in this
file

LMB, MMB, RMB - left, middle or right mouse buttons

K - hotkeys list

RMB Menus – context sensitive – place the cursor over the part or
background and then RMB

These are the main steps in order:

Model Import

Keyshot in the labs has the ProE plugin installed and will therefore
recognise native ProE parts and assemblies. Assemblies will keep
the part structure.

Pick Options or Dbl Click on any of the parts to access the

Options window. In the Scene tab you can manage the parts in
the scene.

If your ProE model does not import correctly there could be a

number of reasons:

Does the assembly import with the parts incorrectly oriented?

Check your constraints in the ProE assembly, if the parts are not
fully constrained or there are ambiguous constraints then KeyShot
may misinterpret their relative position.

Are construction surfaces showing in the model? Make sure any

unwanted surfaces are hidden on a layer.

If all else fails, which it sometimes will in the world of 3D

import/export, from ProE, Save As a neutral model format such as
Step.

Merge with current scene - select this option when you want to add
multiple models into the same scene. You may need to move the
existing object first so the newly imported object doesn’t overlap it -
see below.

Model Orientation

If you’re lucky your model will import in the correct orientation, if

not…..

Options > Scene tab > pick the part/asm name at the top of the
tree

Use the rotation increase/decrease arrows to rotate the model and

then the Snap to Ground option.

Shft + Alt + LMB - move the model off the centre on the ground
plane
Camera Position

In rendering software, visualise the camera position moving rather

than the model moving – we are viewing a scene.

Alt + LMB - Tumble the camera around the focal point

Alt + MMB - Pan the camera

Alt + RMB – Zoom or ‘Dolly’ the camera

Applying Materials

Open the Materials library, simply drag and drop onto the model.

Dbl click a part or RMB (over the part) > Edit Material to edit the
Material properties

Textures

These are pixel based images which over ride the Material. Access
through the Texture tab in the Material properties.

Bump Maps

See CAD/CAM Pages > Rendering > Bumpmaps

Bumpmaps give the impression of a textures surface by adjusting

the surface normals. There are some bumpmaps in the Materials
library under the Texture tab.

Labels
You need to use a tiff with transparency layers to create a see
through ’label’, and move it on the model to see it when you first
apply.

Liquid in Glass Setup

The image at the top this page took some input from some experts
to get up and running as this was my initial result:

First suggestion was to put a tiny gap between the glass container
model and the liquid model. This worked fine and produced this
image:
But the gap in the model above means there is no glass air interface
- the light travels from liquid to air then from air to glass. The input
back from this was that for maximum realism the model should be
created not with a gap but with 3 surfaces;

 the glass air interface - liquid top surface

 the glass air interface
 the glass liquid interface

Download the file below HERE

This was from the KeyShot guys:

" That does look good, but it is still a bit off due to the small gap
you had to create. The reason you need to set up this model like the
wine glass is to be able to pull the refraction of the liquid inside the
glass to the very edge of the outer glass surface. Being able to see
the thickness of the glass surface like this is incorrect.

This file is already set up for proper "liquid-in-glass" rendering and it

shows the important steps beyond just having 3 surfaces to
represent the varying "interfaces" between liquid, air, and glass.

Splitting up the surfaces in this way is important because you need

to set different "IOR" and "IOR out" settings for each of the surfaces.

The IOR is the index of refraction for the "inside" of the surface, and
IOR out is for the "outside" of the surface.

So, looking at the wine glass bip file we do see that there are three
surfaces. The outer most surfaces covers most of the glass itself and
you'll find the material is a solid glass with an IOR of 1.5. This means
the inside of the surface will refract light like glass since glass
typically has an IOR of 1.5. The IOR out for this part would be just 1,
since the outside of the surface should refract like air (no refraction)
and air has an IOR of 1.

That's the easy surface, the next surface, the top of the liquid is
similar. You need to have the inside of the surface represent the
liquid and the outside should represent air. So, for the wine glass
the top of the liquid has an IOR of 1.33 (the IOR of water) and an
IOR out is 1 since it is, again, air.

The third surface, the "interface" of the liquid meeting the glass is
the tricky one. On the inside of the surface you have the liquid, and
the outside you have glass. So, for the wine glass you will see that
this surface has an IOR of 1.33 since the liquid is on the inside, and
an IOR out of 1.5 since glass is on the outside.

You can get even more complicated by applying the same technique
to the color settings of the dielectric material to create proper
colored liquid and colored glass renderings.

Here is my rendering of the wine glass that has these techniques

applied, notice the accurate refraction of liquid within the glass. Just
like the real photo above.

Alias ImageStudio - Quick Guide.

ImageStudio [IS] will import the common neutral file formats STEP, IGES and STL. Either
an individual part file or an assembly can be imported. A STEP from a ProE assembly will
retain its individual part identity allowing easy selection of whole parts.

File > Import Model to bring in your neutral file.

Use Alt + left, right or middle mouse buttons to tumble, zoom or pan the model.

Use the Groups window to easily navigate through and select parts or surfaces in the model.
Expand the assembly groups and use Ctrl to select multiple items.

Use the Asset Library to import environments and materials.

Environment

Simply drag and drop into the model window - soft Lighting > Skylight is a good starting
environment. Check out all the different environment controls. Turn on Cast Shadows.

Through Set Floor Position > Move to Bottom of Model adjust the floor height relative to
the model.

Use the above icon to position your model relative to the environment. Double click the drag
handles to move in defined increments.

Materials

Materials are managed from the Asset Library

Either - select the part or surface and then drag and drop the material directly onto the
selection,

or - drag and drop them into the asset list window on the right and then, from there, drag and
drop them onto a selection.

Both Environments and Materials in the can be modified - colours changed, new light
added, etc

Render

When you have your environment and materials set you will need to consider a test render.
Use the above icon to show the render window above the model window.

Use the Adjust Quality setting to experiment with the Test and Final render output

Resolution

Think carefully about what your doing with the final image - A4 or A0? Web or display
board? Do you really need a very high resolution image?

Your final output is a bitmap image - .jpg, .tif, etc - if this starts to get much above 10Mb then
it can become more problematic to handle and slow to process in print queues.
Set the image size and run a test render. Adjust the image in the model window and Refresh
the rendered image.

Perspective

If you are zoomed in on your model and it is distorted due to the perspective setting then
adjust from Wide angle to Telephoto through Edit > Perspective.

Tessellation

If your model is rendered with very faceted edges then you may need to change the
Tessellation settings.

Drag a box or through the Groups window, select all the objects - the whole assembly, Edit >
Set Per Object Tessellation.

Running ProE on your personal computer

*** After installation but before you start using your own
installation of Creo you need to change it's configuration
files - SEE HERE ***

Hardware Recommendations for Creo Elements Pro 5.0

It is not a course requirement to have your own computer and CAD

software, there is adequate access to PC labs across campus to
complete your coursework. But if you choose to:

Universities Edition – the version used in the computer labs in the

Department - this version uses a network license and therefore
MAY be usable in halls depending on your location.

Student Edition – the version which can be purchased for

standalone home use and does not require a network license.

Spec that will run Creo will run most other 3D software – modelling
or rendering – and will run 2D bitmap and vector graphics software.
Talk to year 2 and year 3 students about what they would
recommend.

Laptop or Desktop?
There is generally no need to bring a laptop into the Department.
So unless you really need the extra portability and compact size
then desktop PCs will give you better value for money and
adaptability.

LCD screens and compact towers give lots of space flexibility. You
can’t use CAD software without a 3 button mouse [scroll wheels
double as middle button].

If you are going for a laptop [or more accurately a ‘mobile desktop’
when it comes to something that will run 3D software] then make
sure its right – laptop are very difficult and expensive to upgrade.

Recommended spec:
Operating System: Windows XP or higher
CPU/processor speed: 2.0GHz
Available hard disk space: 1.5 Gb
RAM memory: 1Gb [recommended: as much as you can afford!]
Graphics card: 128Mb OpenGL compliant

The quality and manufacturer of your graphics card is the main

hardware issue - Pro/E is unlikely to run on systems that have only
‘on board’ graphics. A separate graphics card with a minimum of
64Mb memory [again, recommended is as much as you can afford!]
from nVidea, ATI, PNY is likely to be OK – no guarantees.

Macs – people are running ProE on Macs with Windows emulators

– ask around 2nd/3rd years and look on the Web

Educational Edition

The version of Creo installed on any of the networked lab machines is referred to as the
Educational Edition. It is the version licensed to selected universities which has a full set of
Creo modules.
This version can be installed and run on your personal computer if you are in halls and your
computer is on the university network. Installation disks can be loaned, free of charge, from
the Departmental store. The software uses a network license, therefore it will not run if you
unplug your computer from the network.

Computing services can give you information on setting up your computer to connect to the
network.

** Instructions for installing the Educational Edition can be found here **

Student Edition

You can also purchase a version of Creo which is independently licensed and does not need
your computer to be connected to the network. This is referred to as the Student Edition.
Although the student version has a limited number of modules, those which it does have allow
you to do advanced modelling.

This version can be purchased from ptc.com

Assistance for Student Edition installation (.pdf) be found on the disks along with an
assistance email address.

Converting Units

If you started a new ProE file without the appropriate configuration file active then it is likely
that you part will be in the factory default units - inches. This doesn't make an awful lot of
difference whilst your modelling [although there are accuracy/tolerance issues] the main
issue for this is that in reality your part will be 25.4 times bigger than it should be!

If you bring it into an assembly of parts which are in millimetres then then issue will be more
apparent - your parts will not fit together.

This issue is applicable to all types of files, not just .prt files

To change the units of a ProE file:

Edit > Setup > Units

The red arrow shows the current units system. Highlighted is the system you wish to change
to.

Understand and make the right choice in the Changing Model Units window. It is most likely
you want the second option which will effectively scale your model.