Unit 3 - Drawing

Views
Unit & Lesson Slides
Learning Objectives

This unit is designed to give students an understanding of drawing views. Not only the
various types of views but also how they are created and what they are used for when
creating a drawing. At the end of this unit, students should be able to:
1. Create orthogonal views.
2. Create non-orthogonal views.
3. Understand the difference between ANSI and ISO standards and projection.
4. Create regular section views.
5. Create aligned section views.
6. Create broken-out section views.
7. Create detail views.
8. Create broken views.
9. Recognize when an auxiliary view is needed.
10. Create auxiliary views with the appropriate true shape and size projections.
Key Concepts
Drawing Views
Views are the fundamental element of drawings. Documenting a
3-dimensional object in 2 dimensions requires multiple views. In
technical drawings, these views must portray the object in “True
Shape & Size”. This means that when the drawing scale is 1:1
(actual size), measurements can be taken directly from the
drawing. All the lines and arcs must be exactly the same size as
they are defined to be. In order to do this, orthogonal views must
be used.

The orthogonal views must be dimensioned so that the object in

the drawing could be recreated in a CAD system or manufactured. Isometric view
This means that all pertinent dimensions must be provided on the
drawing and, since orthogonal views are the only ones that can
show true shape and size, all dimensions must be on orthogonal
views.

Other views can be used to portray what the part looks like
3-dimensionally. These views are often called isometric, dimetric
or trimetric depending on the rotations used to create them. Orthogonal views

It is good practice to only include views necessary to

communicate your design.
Sample drawing from Onshape
In this unit we will explore the various kinds of views and how they
are created in Onshape.
Orthogonal Views
Standard Orthogonal Views
When a part is modeled, it is oriented with
respect to an origin and the three standard
orthogonal planes, (Front, Top, Right). Drawing
views are projections from this beginning
orientation. It is therefore important to make
sure the model is oriented with respect to
these planes.

Standard orthogonal planes

Right plane orientation - Right side view

Orthogonal Views Top

Orthogonal views are projections of an object

onto planes oriented parallel to the standard
Front, Top and Right planes. It is like having a
transparent box around the object and
projecting the views onto the surfaces of the
box.

Obviously not all lines or edges are shown in

these views since some of them are hidden by Front
the surfaces of the object that are in front. This
is actually why multiple views are needed,
since parts of the 3-dimensional object are
hidden in any given view.
Right
90 degree
The hidden parts are often shown in the views
rotations
with dashed or grayed-out lines to represent
the fact that they are behind and therefore
hidden. Orthogonal views
Projections & Standard Views
Projections are important in creating the views on a drawing. We’ve discussed how views are created from orthogonal projections onto the
transparent faces of a box that encloses the object. But where you, as the viewer, are, either outside the box or inside the box makes the
views appear differently.

There are two main ways of projecting views; first angle projection and third angle projection. In first angle projection, the viewer is inside
the box and so the object is between the viewer and the screen, (think of it as first person projection since the object is right in front of
you). In third angle projection, you are outside the box and so the screen is between you, the viewer, and the object, (Think of this as third
person projection since the screen is between you and the object).

This may be a little confusing. Why not just pick one way of projecting as the standard way to project? It turns out that there are agencies
that specify drawing standards. One agency is the American National Standards Institute (ANSI) and another is the International Standards
Organization (ISO). ANSI standard drawings use 3rd angle projection and ISO standard drawings use 1st angle projections.

When creating the standard views for a drawing, it is important to choose which type of projection you will use, either ANSI or ISO. The
drawing format for each has a box where the projection method is specified.

3rd angle projection

(3rd person projection)
1st angle projection
(1st person projection)
First Angle Projections
Drawings are 2-dimensional representations of
3-dimensional objects. Since they lack the 3rd
dimension, it is necessary to create multiple views.

There are a set of standard views that are used in

most drawings. In first angle projection, these
standard views can be thought of as the views you Right Side Front
would get if you encased the part in a glass box and
projected the 2 dimensional silhouettes of the part
onto the inside of the glass sides of the box.

Most drawings only require 2-3 of these views to fully

dimension and define the part. However, picking
which 2 or 3 is important.

Another important part of views in drawings is that

they must be aligned with respect to each other so Top
that they represent a 90-degree rotation. These
standard views cannot be randomly placed on the
drawing sheet.
Third Angle Projections

In Third angle projections, these standard views

can be thought of as the views you would get if
you encased the part in a glass box and projected
the 2 dimensional silhouettes of the part onto the
outside of the glass sides of the box.

Selecting the correct views depends on the object

and what views would best document it. Some Top
dimensions can only be placed in certain views.

In order to fully dimension a part it is often

necessary to have more than 3 views. You can add
more of the standard orthographic views or you
can add auxiliary views, partial views, or section Front
views. We’ll talk about each of these in this unit. Right Side
Standard views
Once the projection method has been chosen, the set of views must be chosen. Typically, the Front, Right and Top
views are used. It is important to place these projected views in their correct orientation relative to one another, as
seen below. Depending on the object, other views can be used so that dimensions can be placed appropriately.

The isometric pictorial

view is added for clarity,
but no dimensions can
be added to this view
Non-Orthogonal Views
Pictorial views
Because in 2-dimensional views, only orthogonal projections can produce true shape and size,
orthogonal views are the only views that can have dimensions. However, additional views can be
used for clarity by showing what the part looks like in 3 dimensions. These additional views are
referred to as “Pictorial views,” since they are not orthogonal projections.

Some examples of pictorial views are: Isometric, Trimetric, Dimetric, and Oblique

Isometric views are equal angle rotations about all three axes. Trimetric are views where the object
is rotated in unequal angles about 3 axes. Dimetric are views where the object has been rotated Perspective
about 2 axes, and oblique are arbitrary rotations.

Perspective projection can be added to any of these orientations to make the models look like they
would in the real world. These views can be line drawings or fully shaded.

Oblique

Isometric Trimetric Dimetric

Special Orthogonal Views
Special Views
Because part geometry can be very complex, it is sometimes necessary to create special orthogonal views so that the
part drawing can be fully dimensioned. The special types of view include:
1. Section views
2. Broken-out section views
3. Detail views
4. Broken views
5. Auxiliary views

We will explore each of these views in this section except for auxiliary views which will be discussed in its own section
since these types of views are a little more involved.

Detail view Broken view

Broken section view

Section view
Section Views
Section views provide cross sectional representations so that internal features can be dimensioned and shown.
There are two types of section views: regular section views and aligned section views.

Regular section views are the most commonly used views.

Example of a regular section view Example of an aligned section view

Section Views: Regular
Regular section views have a straight cutting line and the view is projected 90 degrees about the cutting line.

It is important to include the cut line in the adjacent view.

Section Views: Aligned
An aligned section view has an angled cutting line so that the section shows important features that may not be
along a straight cutting line.

In this example, the holes on the round part don’t align with a straight section through the arm, so an aligned
section is used. In the section view both holes can be dimensioned. This may seem strange but it eliminates the
need for multiple section views which could end up being confusing on the drawing.
Broken-out Section Views
A broken-out section view allows a section view to be shown on a portion of a view. This is useful when a
complete section view is unnecessary. It allows dimensions to be placed on the regular view as well as
internal to the part on the broken section view.

Broken section view

Broken section view

Detail views
Step 1: Create regular orthogonal
views. Then identify the view you
Detail views allow clearer definition of a part on a
wish to cut.
drawing by removing unnecessary aspects of the view
and by enlarging a portion of the part to make the
details more obvious.

Step 2: Use the Detail view tool.

Step 3: Select the shape of the

detail view and draw a closed
shape.

Step 4: Click to place the detail

view and Onshape creates the
view.
Broken views
Broken views allow long parts to be foreshortened so that they fit on a regular drawing without unnecessarily long
views.

Best practice is to only shorten continuous surfaces, so the shortening does not hide any features.

The foreshortened views still maintain the correct 3 brakes in the broken view
dimensions.
Auxiliary Views
Auxiliary Views
Some parts have features that aren’t aligned to the standard
orthogonal views and therefore cannot be dimensioned in any
standard view. The features must be documented in auxiliary
views. Top view

Auxiliary views are orthogonal projections that are not standard

views. Auxiliary projections are 90-degree rotations around an
edge that brings a feature into a true shape and size view.
Front view
In the example on the right, the bottom face of the pipe isn’t Right view
orthogonal in any standard view. Notice the holes in the right view
are skewed. In order to get an orthogonal view of this face, we Auxiliary
need to project around the this edge. view

This creates a new auxiliary view where the holes are in true
shape and size and can be dimensioned. In this case you could
eliminate the Right view since the auxiliary view gives you the
ability to dimension the bottom face.
Vocabulary
• Oblique plane = a surface that cannot be dimensioned from normal orthogonal views. It must be
projected to obtain true shape and size.

• True shape and size (TS&S) = the label placed on a view that represents the actual shape and
size of a face of a part after projection.

• True length lines (TL) = True length lines are the only lines in a view that are the actual length of
the side of the part. Any line in a view that is parallel to the projection plane is true length in the
next view.

• Projection lines = the lines that indicate the axis of rotation between views (usually dashed).

• Projection planes = the planes drawn perpendicular to projection lines.

• Edge view = after projecting parallel to a true length line, the following view is the edge view. It
should be a single line.
Single Projection Auxiliary Views
In this example, the part was aligned in such a way that there is an
edge view of the face we need to project. That edge becomes
the projection line around which the view can be rotated.

In this example, the oblique

face is never in an edge view
so it requires that we first
project it into an edge view and
then into a true shape and size
view. This process is explained
in the following slides.
Example: A Simple Oblique Face
Consider a simple example where a cube has a corner cut off to create an oblique face. This face will not be true
shape and size in any of the standard views.

The final
Top View Top view projection is
The first True shape &
projection is around the edge
size view line.
around the true
length line.
Oblique plane

2nd Aux view

The second projection is

around a perpendicular
line to the original true
length line.
1st Aux view

Front view
Front
View

Right side
View
Cube Rotations Thru the Projections
The true length
Imagine the original cube going line is a point.
through each of the projections. True shape &
size projection

Top
View

Oblique plane True length line

Step 1: Project about Step 3: Project

the true length line. around the edge
view of the
oblique face.
Step 2: Project
Front around a line
View perpendicular to the
Right side true length line.
View
Multiple projections Step 4: The 3rd projection gives a true
shape and size view where the holes can be
dimensioned.
Step 1: In order to achieve Step 3: In the second
a true shape and size view, projection, the oblique
we must project 3 times. face is now in an edge
First we project around the view. We can now use the
diagonal line in the top edge as the last
view because it is a true projection line around
shape and size line. which we will get a true
shape and size view.

Step 2: The next view

gives us an edge that is
perpendicular to the
original diagonal line.
We use that to make
the next projection.
Selecting Standard Views: ISO vs ANSI

ISO Drawing (1st angle projection) ANSI drawing (3rd angle projection)

Note: the primary view of a part is usually the most descriptive, or includes
the most important features. Then secondary views are provided for
additional features or information.

The views dialog box in Onshape allows you to customize the preferences for
views. A set of default preferences is loaded when you choose a drawing template.
 Practice
AGENDA
Create a Copy of This Document
For the practice and exercises in this unit, you will need your own editable copy of this document.

Option 1: Click the blue “Make a copy to edit” button at the top of the Onshape interface.

Option 2: Click the main document menu, and select “Copy workspace…”
Creating Views Projected Views:
1. Select the Projected view tool.
Inserting Views:
2. Click an existing view in the drawing.
1. In a drawing, select the
3. Move your mouse away from the initial view (above, to the left,
Insert view tool.
below, etc).
2. Left-click in the drawing to
4. Left-click to place the new view.
place it.
Creating Regular Section Views

Step 1: First, place a regular orthogonal

view in your drawing.

Step 2: Select the Section view tool,

then select Vertical, Horizontal, or
Angular for the cutting line.

Step 3: Select a
point to orient the
cutting line.

Step 4: Left-click in the drawing to

place the view.
Creating Aligned Section Views
Step 1: First, place a regular orthogonal
view in your drawing.

Step 2: Select the Aligned section

view tool.

Step 3: Select a center point.

Step 4: Select the first cutting line.

Step 5: Select the second

cutting line.

Step 6: Click on one side or the other

of the original view to place the
section view.
Creating Broken-Out Section Views
Step 1: Place a regular orthogonal view in
your drawing and a projected view of this
view.

Step 2: Select the Broken-out Broken section view

section tool.

Step 3: Select spline points that

enclose the area you want to break
out. Step 5: Click the green
check mark and Onshape
Step 4: Select a point on will create the broken-out
the projected view to section.
indicate the depth of the
section view.
Creating Broken Views
Step 1: First, place a regular orthogonal
view in your drawing.

Step 2: Select the Break view tool.

Step 3: Click to indicate where the break should occur on

the part and then specify the gap distance. Onshape will
foreshorten the part in the view.

Note: This part has been

foreshortened 3 times.
Projections in Onshape
Step 1: First, place a regular orthogonal
view in your drawing and identify a true
Onshape provides an auxiliary view tool to length line to project around or an edge
allow you to project around lines or edges in view of the oblique face.
the standard views.
Step 2: Select the Auxiliary view tool.

Step 3: Select the line

around which you wish to
project.

Step 4: Left-click in the

drawing to place the view.
 Examples
AGENDA
Example
Inthis example, the base of the walking robot has a set of
faces, where the legs attach, that are oblique to the TS&S View
orthogonal views.

A series of projections was necessary to obtain a true

shape & size view.

Oblique
faces
Example
The cylinder head for this radial engine has oblique
faces. Two projections are required to get a true
shape and size view.
TS&S View

This is the only

correct dimension.

These dimensions
are not correct for
these lines.
 Exercises
AGENDA
Create a Copy of This Document
If you haven’t already done so, for the practice and exercises in this unit, you will need your own editable copy of this
document.

Option 1: Click the blue “Make a copy to edit” button at the top of the Onshape interface.

Option 2: Click the main document menu, and select “Copy workspace…”
Exercise Objectives
The purpose of these exercises is to give students the opportunity to practice.

The specific skills are:

1. Creating orthogonal views.
2. Creating non-orthogonal views.
3. Explaining the difference between ANSI and ISO standards and projection.
4. Creating regular section views.
5. Creating aligned section views.
6. Creating broken-out section views.
7. Creating detail views.
8. Creating broken views.
9. Recognizing when an auxiliary view is needed.
10. Creating auxiliary views with the appropriate true shape and size projections.
Exercise 1: Orthogonal & Non-Orthogonal
Part 1: Using the Roadster model in this document, create an ANSI drawing and an ISO drawing
with Front, Right and Top views as well as an Isometric view.

Part 2: Use the drawing of the landing gear yoke above to create a model
and then duplicate the drawing.
Exercise 2: Regular Section Views
Part 1: Use the Turbine Strut assembly to create the drawing below. Use the section view
tool to create a regular section view for the right view.

Part 2: Add the pockets indicated in the drawing to the landing

gear yoke to reduce the weight. Now update your drawing with a
regular section view, since you can’t dimension to hidden lines.
Exercise 3: Aligned Section Views
Part 1: Use the HP Casing model in the Turbine Strut assembly to create the
drawing below. Use the aligned section tool to create a section view as shown.

Part 2: Model the brake disc shown in the drawing above

and then create the drawing. Make sure to use an aligned
section view.
Exercise 4: Broken-Out & Detail Section Views
Part 1: Make a drawing of the Turbine Strut Fan Assembly Part 2: Add lubrication holes to the yoke model as
as shown below. Create a broken-out section and then a shown in the drawing and then update your drawing
detailed view of the broken-out section. with a broken-out section and a detail view.
Exercise 5: Broken Views
Part 1: Use the model of the Upper Shock Cylinder in Part 2: Create the Lower Shock Arm as shown in the
the Landing Gear assembly to create the drawing drawing. Then create the drawing with breaks in the arm
below. Use the break section tool to foreshorten the so that the scale is large enough to see the details.
two views as shown.
Exercise 6: Auxiliary Views
Use the model of the Bracket, in the Exercises
folder, and create a drawing with the front and
top views. Then use the auxiliary view tool to
project a true shape and size view as shown.
Check your dimensions with the drawing.
Exercise 7: Auxiliary Views
Document the true length of the side of the orange face on the shrouded turbine blade model in an auxiliary view.
Hint: The orange face is in an edge view in an orthogonal view, so you just need to project around the edge to create
the true shape and size view.

CMC Leopard small business jet engine

Summary
This unit is focused on the many types of drawing views. Not only the various types of views but also
how they are created and what they are used for when creating a drawing.

Unit 4 focuses on dimensioning.