LESSON 3

BASIC PART MODELLING

UPON SUCCESSFUL COMPLETION OF THIS LESSON,
YOU WILL BE ABLE TO:

• Choose the best profile for sketching.

• Choose the proper sketch plane.
• Extrude a sketch as a cut.
• Create Hole Wizard holes.
• Insert fillets on a solid.
• Use the editing tools edit sketch, edit feature and rollback.
BASIC MODELLING

• This lesson discusses the

considerations that you make
before creating a part, and
shows the process of creating
a simple one.
STAGES IN THE PROCESS
THE STEPS IN PLANNING AND EXECUTING THE CREATION OF THIS
PART ARE LISTED BELOW.
• Terminology • Design intent
• What are the terms commonly used when • What is design intent and how does it
talking about modeling and using the affect the modeling process?
SolidWorks software?
• New part
• Profile choice
• Opening the new part is the first step.
• Which profile is the best one to choose when
starting the modeling process? • First feature
• Sketch plane choice • What is the first feature?
• Once you’ve chosen the best profile, how
does this affect your choice of sketch plane?
STAGES IN THE PROCESS
THE STEPS IN PLANNING AND EXECUTING THE CREATION OF THIS
PART ARE LISTED BELOW.

• Bosses, cuts and hole features • Drawings

• How do you modify the first feature • Creating a drawing sheet and
by adding bosses, cuts and holes? drawing views of the model.
• Fillets • Dimension changes
• Rounding off the sharp corners — • Making a change to a dimension
filleting.
changes the model’s geometry.
• Editing tools How does this happen?
• Use three of the most common editing
tools.
TERMINOLOGIES
TERMINOLOGIES
• Feature - All cuts, bosses, planes and sketches that you create are
considered Features. Sketched features are those based on
sketches (boss and cut),and applied features are based on
edges or faces (fillet).
• Plane - Planes are flat and infinite. They are represented on the screen
with visible edges. They are used as the primary sketch surface
for creating boss and cut features.
• Extrusion - An extrusion will extend a profile along a path typically normal
to the profile plane for some distance. The movement along that
path becomes the solid model.
TERMINOLOGIES
• Sketch - In the SolidWorks system, the name used to describe a 2D
profile is sketch. Sketches are created on flat faces and planes
within the model. They are generally used as the basis for bosses
and cuts, although they a can exist independently.
• Boss - Bosses are used to add material to the model. The critical initial
feature is always a boss. After the first feature, you may add as
many bosses as needed to complete the design. As with the base,
all bosses begin with a sketch.
• Cut - A Cut is used to remove material from the model. This is the
opposite of the boss. Like the boss, cuts begin as 2D sketches and
remove material by extrusion, revolution, or other methods you
will learn about.
TERMINOLOGIES
• Fillet & Rounds - Fillets and rounds are generally added to the solid, not
the sketch. By nature of the faces adjacent to the
selected edge, the system knows whether to create a
round (removing material) or a fillet (adding material).
• Design Intent - How the model should be created and changed, is
considered the design intent. Relationships between
features and the sequence of their creation all contribute
to design intent.
•
BEST PROFILE

• Choosing the Choose the “best” profile. This profile, when

extruded, will generate more of the model than any other.
LOOK AT THESE MODELS AS EXAMPLES

Part Best Profile Extruded

LOOK AT THESE MODELS AS EXAMPLES

Part Best Profile Extruded

LOOK AT THESE MODELS AS EXAMPLES

Part Best Profile Extruded

LOOK AT THESE MODELS AS EXAMPLES

Part Best Profile Extruded

LOOK AT THESE MODELS AS EXAMPLES

Part Best Profile Extruded

CHOOSING THE SKETCH PLANE
• Once the best profile is determined, the next step is to decide which view to
use and select the plane with the same name for sketching it. The SolidWorks
software provides three planes; they are described below.

Planes There are three default planes, labeled Front Plane, Top Plane and Right
Plane. Each plane is infinite, but has screen borders for viewing and selection.
Also, each plane passes through the origin and is mutually perpendicular to
the others.
The planes can be renamed. In this course the names Front Plane, Top Plane
and Right Plane replace the default names respectively. This naming
convention is used in other CAD systems and is comfortable to many users.
Although the planes are infinite, it may be easier to think of them as forming
an open box, connecting at the origin. Using this analogy, the inner faces of
the box are the potential sketch planes.
CHOOSING THE SKETCH PLANE
• Once the best profile is determined, the next step is to decide which view to
use and select the plane with the same name for sketching it. The SolidWorks
software provides three planes; they are described below.

Placement of The part will be placed into the box three times. Each time the best profile
the Model will contact or be parallel to one of the three planes. Although there are
many combinations, the choices are limited to three for this exercise.
There are several things to consider when choosing the sketch plane. Two are
appearance and the part's orientation in an assembly. The appearance
dictates how the part will be oriented in standard views such as the Isometric.
This also determines how you will spend most of your time looking at the
model as you create it.
The part's orientation in an assembly dictates how it is to be positioned with
respect to other, mating parts.
CHOOSING THE SKETCH PLANE
• Once the best profile is determined, the next step is to decide which view to
use and select the plane with the same name for sketching it. The SolidWorks
software provides three planes; they are described below.

Orient the Model Another consideration when deciding which sketch plane to use
for the Drawing is how you want the model to appear on the drawing when
you detail it. You should build the model so that the Front view
is the same as the Front view will be in the final drawing. This
saves time during the detailing process because you can use
predefined views.
CHOOSING THE SKETCH PLANE
CHOOSING THE SKETCH PLANE
TOP PLANE FRONT PLANE RIGHT PLANE
CHOOSING THE SKETCH PLANE
TOP PLANE FRONT PLANE RIGHT PLANE

The Top plane orientation seems to be the best. This indicates that the
best profile should be sketched on the Top plane of the model.
PROCEDURE
• The process in this lesson includes sketching and extrusions. To begin
with, a new part file is created.

INTRODUCING NEW PART

• The New tool creates a new SolidWorks document from a selection
of part, assembly or drawing templates. There are several training
templates in addition to the default ones.

WHERE TO FIND IT
• From the File menu, select New.
• Or, on the Standard toolbar, click New (J).
EXAMPLE
DETAILS OF THE PART
• The part we will be creating is shown below.

Front View Rear View

DETAILS OF THE PART
• The part we will be creating is shown below. There are two main boss
features, some cuts, and fillets.

Front View Rear View

STANDARD VIEWS
• The part is shown here in four standard views.
MAIN BOSSES

• The two main bosses have distinct

profiles in different planes. They are
connected as shown in the exploded
view at right.
BEST PROFILE
• The first feature of the model
is created from the
rectangular sketch shown
overlaid on the model. This is
the best profile to begin the
model.
• The rectangle will then be
extruded as a boss to create
the solid feature.
PROCEDURE
STEP 1: NEW PART

• ClickNew, or click File, New.

Create a new part using the
Part_MM template and Save it
as Basic.
STEP 2: ANNOTATIONS SETTING

• Right-click
the Annotations folder and clear the Automatically
Place into Annotation Views option. This will prevent dimensions
from being inserted with drawing views later in the lesson.
STEP 3: SELECT THE SKETCH PLANE

• Observe what sketch plane to use?

STEP 3: SELECT THE SKETCH PLANE

• Selectthe sketch plane. Insert a new

sketch and choose the Top Plane.
STEP 4: SKETCH A RECTANGLE

• Click the Corner

Rectangle tool and
begin the rectangle
at the origin.

Make sure the rectangle is locked to the origin by looking for the
vertex cursor as you begin sketching. Do not worry about the size of
the rectangle. Dimensioning it will take care of that in the next step.
STEP 5: FULLY DEFINE A SKETCH

• Add dimensions to the sketch.

The sketch is fully defined.
EXTRUDE OPTIONS

• End Condition Type

• A sketch can be extruded in one or two directions, Either or both directions can
terminate at some blind depth, up to some geometry in the model, or extend
through the whole model.

• Depth
• The distance for a blind or mid-plane extrusion. For mid-plane, it refers to the
total depth of the extrusion. That would mean that a depth of50mm for a mid-
plane extrusion would result in 25mm on each side of the sketch plane.

• Draft
• Applies draft to the extrusion. Draft on the extrusion can be inwards(the profile
gets smaller as it extrudes) or outward.
STEP 6: EXTRUDE

• Click Extrude and extrude the

rectangle 10mm upwards.
• Click OK.
FINISHED 3D MODEL

• The completed feature is shown

at the right.
STEP 7: RENAME THE FEATURE

• Itis good practice to rename the features that you create with
some meaningful name. In the Feature Manager design tree, use
a very slow double-click to edit the feature Extrude1. When the
name is highlighted and editable, type BasePlate as the new
feature name. All features in the SolidWorks system can be
edited in the same way.
SKETCHING ON A PLANAR FACE

• Any planar (flat) face of the model can be used as a sketch plane.
Simply select the face and choose the Sketch tool. Where faces
are difficult to select because they are on the rear of the model or
are obscured by other faces, the Select Other tool can be used to
choose a face without reorienting the view. In this case, the planar
face on the front of the BasePlate is used.
STEP 8: INSERT NEW SKETCH

• Create a new sketch using

insert, Sketch or by clicking the
Sketch tool. Select the
indicated face.
STEP 9: VERTICAL LINE

• Click the line tool and start the

vertical line at the lower edge
capturing Coincident relation at
the lower edge and Vertical
relation.
STEP 10: AUTO-TRANSITIONING

• Press the letter A on the keyboard.

• You are now in tangent arc mode.
STEP 11: TANGENT ARC

• Sketch a 180° arc tangent to the

vertical line. Look for the inference
line indicating that the end point of
the arc is aligned horizontally with
the arc’s center.
• When you finish sketching the
tangent arc, the sketch tool
automatically switches back to the
line tool.
STEP 12: FINISHING LINES

• Create a vertical line from the arc

end to the base, and one more line
connecting the bottom ends of the
two vertical lines.
• Note that the horizontal line is black,
but its endpoints are not.
STEP 13: ADD DIMENSIONS

• Add linear and radial dimensions to

the sketch.
• As you add the dimensions, move the
cursor around to view different
possible orientations.
• Note: Always dimension an arc by
selecting on its circumference, rather
than center.
STEP 14: EXTRUDE DIRECTION

• Click insert, Boss, Extrude and set the

Depth to 10mm. Note that the
preview shows the extrusion going
into the base, in the proper
direction.
• Note: If the direction of the preview
is away from the base, click the
Reverse direction button.
STEP 15: COMPLETED BOSS
• The boss merges with the previous base to form a single solid.
• Rename the feature VertBoss.
CUT EXTRUDE

• The menu for creating a cut feature by extruding is

identical to that of creating a boss. The only difference is
that a cut removes material while a boss adds it. Other
than that distinction, the commands are the same. This cut
represents a slot.
STEP 16: CREATE A RECTANGLE

• Press the spacebar and double-click

*Front. Start a sketch on this large
face and add a rectangle
Coincident with the bottom model
edge.
• Turn off the rectangle tool.
STEP 17: RELATIONS

• Add a dimension as shown.

Change the view orientation to
Isometric.
STEP 18: THROUGH ALL CUT

• Click insert, Cut, Extrude or pick the

Extruded Cut tool From on the
Features toolbar. Choose Through All
and click OK. This type of end
condition always cuts through the
entire model no matter how far. No
depth setting was needed.
• Rename the feature BottomSlot.
USING THE HOLE WIZARD

• The Hole Wizard is used to create specialized holes in a solid. It

can create simple, tapered, counterbored and countersunk holes
using a step by step procedure. In this example, the Hole Wizard
will be used to create a standard hole.
USING THE HOLE WIZARD

• Creating a Hole - You can choose the face to insert the hole onto, define the
hole’s dimensions and locate the hole using the Hole
Wizard. One of the most intuitive aspects of the Hole
Wizard is that you specify the size of the hole by the
fastener that goes into it.
• Tip - You can also place holes on planes and non-planar faces.
For example, you can create a hole on a cylindrical face.
• The Hole Wizard - The Hole Wizard creates shaped holes, such as
countersunk and counterbore types. The process creates
two sketches. One defines the shape of the hole. The
other, a point, locates the center.
STEP 19: HOLE POSITION

• Select the face indicated and Insert,

Features, Hole, Wizard....
STEP 20: SELECT COUNTERBORE
Set the properties of the hole as
follows:
• Type: Counterbore
• Standard: Ansi Metric
• Type: Hex Bolt
• Size: M8
• End Condition: Through All

Click the Positions tab.

STEP 21: WAKE UP THE CENTERPOINT
• Turn on the Point tool. Drag the point onto the
circumference of the large arc. Do not drop it.
• When the Coincident symbol appears, the
center point of the large arc has been “woken
up” and is now a point you can snap to.
• Drop the point onto the arc’s centerpoint. Look
for the feedback that tells you that you are
snapping to the arc’s center, a coincident
relation. Click OK to add the relation and
again to complete the dialog.
FILLETING

• Filleting refers to both fillets (adding volume) and rounds (removing volume).
The distinction is made by the geometric conditions, not the command itself.
Fillets are created on selected edges. Those edges can be selected in several
ways. Options exist for fixed or variable radius fillets and tangent edge
propagation.
FILLETING RULES

• 1. Leave cosmetic fillets until the end.

• 2. Create multiple fillets that will have the same radius in the same command.
• 3. When you need fillets of different radii, generally you should make the
larger fillets first.
• 4. Fillet order is important. Fillets create faces and edges that can be used to
generate more fillets.
STEP 22: INSERT FILLET

• The Fillet options appear in the

PropertyManager. Click Manual and
set the radius value.
• Radius = 8mm
STEP 23: EDGE SELECTION

• The edges will highlight as the cursor

moves over them and then appear
blue as they are selected. Edges are
automatically filtered by the Fillet
command.
• A callout appears on the first edge
you select. Select six edges total
and click OK.
STEP 24: COMPLETED FILLETS

• All six fillets are controlled by the

same dimension value. The creation
of these fillets has generated new
edges suitable for the next series of
fillets.
STEP 25: RECENT COMMANDS

• SolidWorks provides a “just used”

buffer that lists the last few
commands for easy reuse.
• Right-click in the graphics area and
select Recent Commands and the
Fillet command from the drop-down
list to use it again.
STEP 26: PREVIEW AND PROPAGATE

•A selected edge that connects to

others in a smooth fashion (through
tangent curves) can propagate a
single selection into many.
• Add another fillet, radius 3mm,using
Full preview. Select the edges
indicated to seethe selected edges
and preview.
EDITING SKETCH

• Edit Sketch enables you to access a sketch and make changes to

any aspect of it. During editing, the model is “rolled back” to its
state at the time the sketch was created. The model will be rebuilt
when the sketch is exited.
STEP 27: EDIT THE SKETCH

• Right-click the BottomSlot feature and select Edit Sketch. The existing sketch
will be opened for editing.
STEP 28: RELATIONS

• Select the endpoint and edge as

shown and add a Coincident
relation.
STEP 29: REPEAT STEP 28

• Repeat the procedure for the end

pointat the other end of the
rectangle as shown. The addition of
these relations will fully define the
sketch.
STEP 30: EXIT THE SKETCH

• Click Exit Sketch & in the upper right (confirmation) comer to exitthe sketch
and rebuild the part.
EDITING FEATURE

• Edit Feature changes how a feature is applied to the model. Each

feature has specific information that can be changed or added to,
depending on the type of feature it is. As a general rule, the same
dialog box used to create a feature is used to edit it.
STEP 31: EDITING THE FEATURE

• Right-click the Fillet feature and select Edit Feature. The existing feature will
be opened for editing using the same Property Manager that was used to
create the feature.
STEP 32: SELECT ADDITIONAL EDGE

• Selectthe additional edge as

shown and the propagation will
create the fillets as shown. Click
OK.
ROLLBACK BAR
• The Rollback bar is the blue horizontal bar located at the bottom of the
Feature Manager design tree.
• Itis a tool that has many uses. It can be used to “walk through” a model
showing the steps that were followed to build it or to add features at a
specific point in the part’s history. In this example, it will be used to add a hole
feature between the existing fillet features.
• You can roll back a part using the Rollback Bar in the Feature Manager
design tree. The rollback bar is a line which highlights when selected. Drag the
bar up or down the Feature Manager design tree to step forward or
backward through the regeneration sequence.
STEP 33: ROLLBACK
• Click on the Rollback bar and drag it upwards. Drop it between the fillet features as
shown.
STEP 34: HOLE WIZARD

• Click the Hole Wizard tool and click

the Positions tab.
STEP 35: SELECT FACE

• Select the top, flat face of the base

feature near the location shown.
• Tip Multiple instances of the hole can
be created in one command by
inserting additional points at other
locations.
STEP 36: A SECOND HOLE

• Float over the arc edge to “wakeup”

the centerpoint. Place the point at
the centerpoint.
STEP 37: MOVE FIRST HOLE

• Using the same procedure, drag the

first point to the centerpoint on the
opposite side.
STEP 38: TYPE
Click the Type tab. Set the properties of
the hole as follows:
• Type: Hole
• Standard: Ansi Metric
• Type: Drill sizes
• Size: 7.0
• End Condition: Through All
Click OK.
STEP 39: CHANGE THE VIEW ORIENTATION

• Click Isometric to change view

orientation.
STEP 40: ROLL TO END
• Click on the rollback bar and right-
click Roll To End.
INTRODUCING APPEARANCE

• Edit Feature changes how a feature is applied to the model. Each

Use Appearances to change the color and optical properties of
graphics. Color Swatches can also be created for user defined
colors.
STEP 41: APPEARANCE

• Right-click the top level feature and

choose Appearances and the 2 Ton
Plane name Basic.
STEP 42: SELECT SWATCH
• Under the Color selection, select the standard
swatch and one of the colors as shown.
• Click OK.
STEP 43: SAVE THE RESULTS

• Click Save on the Standard toolbar, or click File, Save to save your work.
EXERCISE 3.1: PLATE
• Create this part using the information and dimensions provided. Sketch and
extrude profiles to create the part.
EXERCISE 3.2: CUT

• Use rectangles, tangent arcs and cut features to create the part.
EXERCISE 3.3: BASIC CHANGES

• Make changes to the part created in the previous lesson.

EXERCISE 3.4: BASE BRACKET

• Create the part below.

END OF LESSON 3

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