Molds design in solid works

Molds Design Introduction
In this lesson, you create a mold tooling for a telephone handset.
You start with a model of a telephone handset. Before creating the mold tooling, you add
mounting bosses to the model. This demonstrates the fastening features commonly used
on molded products.
Then you create the mold, which is composed of a core and cavity. The core duplicates
the inner surface of the model, and the cavity duplicates the outer surface of the model.
A parting surface divides the core from the cavity.
To manufacture the telephone handset, the core and cavity are joined together, and liquid
plastic or metal is injected to fill the open areas between the core and the cavity. After the
liquid cools and solidifies, the core and cavity are separated, and the part is ejected.
Before you create the core and cavity, you prepare the model using the tools listed below,
to ensure that the part will eject properly.
Draft Analysis Shut-off Surfaces
Undercut Analysis Parting Surfaces
Draft Tooling Split

Scale Core
Parting Lines
Starting model - courtesy of Marcelo Nicosia Isometrix Design, Inc.
Core and Cavity
I. Opening the Model
Open telephone.sldprt, then save it with a new name so the original model is still available
if needed.
1. Open telephone.sldprt (browse to drive letter:UsersPublicPublic
DocumentsSOLIDWORKSSOLIDWORKS
versionsamplestutorialmoldstelephone.sldprt).

2. Click View > Display and clear RealView Graphics to optimize your
computer's performance for the complex calculations required to create molds.
3. Save the part as MyTelephone.sldprt.
II. Inserting Mounting Bosses
First, you add mounting bosses to the part.
1. In the FeatureManager design tree:
a. Expand Boss-Extrude1.
b. Click Sketch14 and select Show .
2. Click Mounting Boss (Fastening Feature toolbar) or Insert > Fastening Feature >
Mounting Boss.
3. Select the face as shown for Select a face or a 3D point . This is where the mounting
boss will be placed.
4. In the graphics area, select the following:

a. The circular sketch for Select circular edge to position the mounting boss
.
b. The top face of Boss-Extrude1 for Select Direction.
Select a top face and not an edge. If you select an edge, right-click the selected
edge of Boss-Extrude 1 part and click Select Other to select the top face from
the list. You can also press F5 and click Filter Faces (Selection Filter toolbar)
to restrict selection to faces only.
5. In the PropertyManager, under Boss Type, select Pin Boss and click Hole .
6. In the PropertyManager, under Boss:
a. Set B: Enter diameter of the boss to 5.
b. Click Select mating face, then select the top face of the boss as you did in step
4. This creates the mounting boss at the same height as the boss.
c. Set C: Enter draft angle of the main boss to 1.
d. Set E: Enter height of the hole/pin to 20.
7. Under Fins, set Enter number of fins to 0.
8. Click .
9. Repeat steps 2 through 8 to create a second mounting boss on the opposite end of the
phone as shown.

III. Mirroring the Mounting Bosses
Now that you have two mounting bosses, you can mirror them to create two more.
1. Click Plane (Reference Geometry toolbar).
2. For First Reference, in the graphics area, select the point as shown.
3. For Second Reference, in the flyout FeatureManager design tree, select the Front plane
and click .
A plane is created parallel to the Front plane through the selected point. You can mirror
the mounting bosses about this plane.

4. In the FeatureManager design tree, right-click Sketch14 and select Hide .
5. Click Mirror (Features toolbar).
6. In the flyout FeatureManager design tree, select:
a. Plane9 for Mirror Face/Plane .
Use the vertical scroll bar to view Plane9 at the bottom of the tree.
b. The two mounting bosses for Features to Mirror .
7. Click .
The mounting bosses are mirrored to the other side of the part.
IV. Checking for Draft
Now that the model is complete, you can start to create the mold. First, verify that all faces
include sufficient draft with the Draft Analysis tool. (Draft is a slight taper on selected
model faces that facilitates removal of the part from the mold tooling.)
You can use the Parting Line tool to check for draft and apply the parting lines in a
single step. However, with some complex models, adding draft after you create the
parting lines can cause changes to the geometry that require you to re-apply the parting
lines.

Another method is to use Draft Analysis , which includes functionality not found in the
Parting Line tool, such as displaying a count for each type of face on the model. Then, if
needed, add draft using Draft (for models created in SOLIDWORKS) or tools such as
Ruled Surface or Replace Face on the Surfaces toolbar (for imported models).
Finally, use Parting Line to add the parting line.
1. Click Isometric (Standard Views toolbar).
2. Click Draft Analysis (Mold Tools toolbar).
3. Select the Top plane in the FeatureManager design tree for Direction of Pull in the
PropertyManager.
If necessary, click Reverse Direction so the preview arrow points up.
For Direction of Pull, you can select a linear edge or any other entity that specifies a
vector. When you select a plane or planar face, the direction is normal to the selected
entity.
4. Under Analysis Parameters:
a. Set Draft Angle to 0.5.
b. Select Face classification.
5. Click Rotate View (View toolbar) to see the faces with negative draft.

V. Completing the Draft Check
Under Color Settings, each face type displays a count.
Positive draft Requires draft
Negative draft Straddle faces
 The draft colors shown are the default values. Edited values may display different colors.
 To identify problem faces, hide faces that have correct draft (Positive draft and Negative
draft) by clicking Show/Hide .
1. Click Front (Standard Views toolbar) to examine the lower edge of the model, below
the positive draft.
2. Click Zoom to Area (View toolbar) to magnify the area that requires draft.

The color indicates that these faces have a draft angle less than the 0.5 specified
for Draft Angle .
3. Click .
The analysis results remain visible in the graphics area.
Draft Analysis does not add an item to the FeatureManager design tree.
You can also run Undercut Analysis if the model includes undercut areas (trapped areas
that prevent the part from ejecting from the mold).
Undercut Analysis
The Undercut Analysis tool finds trapped areas in a model that cannot be ejected
from the mold.
For example, suppose the telephone handset has a hole in its side for a cord clip.
Undercut Analysis identifies the faces of the hole as undercut faces. This area requires a
side core. When the main core and cavity are separated, the side core slides in a direction
perpendicular to the motion of the main core and cavity, enabling the part to be ejected.
Hole for cord clip Undercut faces highlighted in red
To run undercut analysis:
1. Click Undercut Analysis (Mold Tools toolbar).

2. In the PropertyManager, set options for Analysis Parameters.
Under Analysis Parameters, you can specify one of the following:
o Direction of Pull. All faces are evaluated to determine if they are visible from
above the part and from below the part. This identifies depressions in the wall of
the part that require a side core.
o Parting Line. Faces above the parting line are evaluated to determine if they are
visible from above the parting line. Faces below the parting line are evaluated to
determine if they are visible from below the parting line. This identifies depressions
in the wall of the part that require a side core, and also helps you to identify sections
of the parting line that you can modify to avoid the need for side cores.
Undercut Analysis identifies four types of undercut faces:
o Direction1 undercut. Faces that are not visible from above the part or parting line.
o Direction2 undercut. Faces that are not visible from below the part or parting line.
o Occluded undercut. Faces that are not visible from above or below the part.
o Straddle undercut. Faces that draft in both directions.
3. Click .
In this case, the hole for the cord clip is identified as an occluded undercut, so a
side core is needed. You create a side core after you create the main core and
cavity.
VI. Adding Draft
Not all faces meet the .5° specified in Draft Angle . Use the Draft tool to add draft to
the faces.
1. Click Draft (Mold Tools or Features toolbar).
2. In the PropertyManager, select Parting Line in Type of Draft.
3. Set Draft Angle to 1.
4. Under Direction of Pull:
a. Select the Top plane in the FeatureManager design tree.
b. If necessary, click Reverse Direction so the preview arrow points down.
Direction of Pull
Direction of Pull defines the direction that the tooling body (cavity or core) is pulled to
separate the mold. It controls the direction in which the draft angle is applied. In this case,

the faces to which you are adding draft are on the core side. Because the core is pulled
down when the mold is separated, the Direction of Pull arrow must point down.
Indicates the parting line
Direction of Pull - incorrect
Direction of Pull - correct
(In these images, an angle steeper than the specified 0.5° was used to make the
difference more pronounced.)
5. Click Dimetric (Standard Views toolbar).
6. For Parting Lines , select each edge along the bottom of the model. You can select
each edge individually, or right-click one edge and click Select Tangency.

7. Click to add the draft.
The draft analysis results update in the graphics area. The thin faces along the bottom
edge become red to show that they now have negative draft.
VII. Applying Scaling
To create the model, liquid plastic is injected into the mold tooling while the mold is closed.
A cooling system in the core and cavity reduces the temperature of the hot plastic.
During cooling, the plastic shrinks. To account for shrink factor, you must scale the model
slightly larger before you create the core and cavity. The shrink factor is a known value
that is based on the type of plastic and the mold conditions. Use the Scale tool to apply
a shrink factor to accommodate for the amount the plastic will shrink as it cools. The Scale
tool scales only the geometry of the model. It does not scale dimensions, sketches, or
reference geometry.
1. Click Scale (Mold Tools toolbar).
2. Expand Solid Bodies(1) in the FeatureManager design tree and select Draft2 as the
Solid and Surface or Graphics Bodies to Scale in the PropertyManager.
The body in Solid Bodies(1) assumes the name of the last feature applied to it.

3. Select Centroid in Scale about.
Scaling about the centroid ensures that all of the geometry is scaled proportionately. A
model's centroid is based on its mass properties. You can display the centroid using the
Mass Properties tool that measures and displays the density, mass, volume, and so on
for the model
4. Select Uniform scaling.
5. Set Scale Factor to 1.05.
6. Click .
VIII. Generating Parting Lines
The Parting Line tool checks draft and adds parting lines. Parting lines separate the core
from the cavity.
About Model Ejection Requirements
 All faces must draft away from the parting line which divides the core from the cavity.
 Design specifications must include a minimum draft angle to test against.
 Cavity side surfaces must display a positive draft.
 Core side surfaces must display a negative draft.
 All surfaces must display a draft angle greater than the minimum specified by the design
specifications.
 No straddle faces must exist.
These requirements ensure ejection of the model from the mold.
1. Click Parting Lines (Mold Tools toolbar).
2. Select the Top plane in the FeatureManager design tree for Direction of Pull in the
PropertyManager.

If necessary, click Reverse Direction so the preview arrow points up.
3. Set Draft Angle to 0.5.
4. Click Draft Analysis to check the model for draft.
Under Parting Lines, the eight edges that define the path of the parting line appear
for Edges . Under Message, a message warns that you might need to create
shut-off surfaces.
If the model includes a closed-loop chain of edges that runs between positive and negative
faces (without straddle faces), the parting line is generated along that chain of edges. (A
chain of edges is a series of connecting edges. If the connecting edges are continuous,
they form a closed loop. You can also have connecting edges that form a partial loop.)
However, a system-generated parting line does not guarantee that all faces have sufficient
draft.
About Straddle Faces
Straddle faces are faces that contain both positive and negative types of draft. Typically,
you need to split a straddle face into two separate faces to prevent the part from being
trapped in the mold. You can split a straddle face:
 Manually, using Split Line (Curves toolbar).

 Automatically, by selecting Split faces in the Parting Line PropertyManager, then
specifying to split at:
o The transition between positive and negative draft
o A specified draft angle
 Manually, in the Parting Line PropertyManager, by selecting vertices, sketch segments, or
splines in the graphics area for Entities To Split .
IX. Completing the Parting Lines
1. Compare the colors on the model with the colors under Mold Parameters.
Positive No Draft Negative Straddle
Upper view. Positive draft
2. Click Rotate View (View toolbar) to examine the flip side of the model.
Lower view. Negative draft
3. Rotate the model and verify that there are no Straddle faces or faces that display
No Draft

The model meets all of the requirements needed to separate the core from the
cavity.
The draft colors shown are the default values. Edited values may display different colors.
To verify the draft type, place the pointer over the color to display the tooltip.
4. Click to create the parting lines.
5. Save the model, rebuilding if prompted.
A Closer Look At Parting Lines
In the Parting Line PropertyManager, you can create parting lines:
 Automatically, as demonstrated in this tutorial. If the model includes a chain of edges that
runs between positive and negative faces (without straddle faces), the parting line is
generated along that chain of edges. Additionally, if the model includes:
o Straddle faces, you can automatically split them, either along the +/- boundary or
at a specified draft angle.
o Multiple chains, the longest chain is selected.
 Manually, using selection tools available in the PropertyManager. While manually creating
a parting line, you can split faces by selecting vertices, sketch segments, or splines in the
graphics area for Entities To Split in the PropertyManager.
Additionally, you can create:

 Multiple parting line features in a single part. For example, you can create parting lines for
shut-off surfaces in addition to the main core/cavity parting line.
 Partial parting line features. This allows you to define a section of the parting line, then
close the PropertyManager. Later, you can edit the parting line feature to close the loop
and complete the definition.
X. Adding Shut-off Surfaces
To cut the tooling block into two pieces, you need two complete surfaces (a core surface
and a cavity surface) without any through holes. Shut-off surfaces close up the through
holes.
The changes to the geometry required to patch so many areas are very complex. Depending on
variables such as your hardware, the number of processes running, and so on, these shut-off
surface operations might require a few minutes to complete.
1. Click Shut-off Surfaces (Mold Tools toolbar).
In the PropertyManager, all the through holes appear in Edges .
2. Under Edges, select the following:
o Knit. Joins each shut-off surface into the cavity and core surfaces.
o Filter loops. Filters out loops that do not appear to be valid holes.
o Show callouts.
In the graphics area, callouts identify each loop with the default surface fill type, Contact.
About Shut-off Surfaces Fill Types
A shut-off surface closes up a through hole by creating a surface patch along a parting
line or edges that form a continuous loop. You can create shut-off surfaces before or after
you create parting lines in a model.
Control the curvature of patches by selecting different fill types (Contact, Tangent, or No
Fill).
Click a callout to change the fill type of a loop from Contact to Tangent to No Fill.
 Contact. Creates a surface within the selected boundary. This is the default type of
surface fill for all loops selected automatically.
 Tangent. Creates a surface within the selected boundary, but maintains the tangency of
the patch to adjacent faces. Click the arrow to change which faces are used for tangency.

Tangent to the walls of the hole:
Tangent to the surface that the hole penetrates:
 In addition to simple loops, use Tangent for more complex through holes, where
the software collects pairs of edges and constructs and knits together a series of
planar surfaces.
Complex through hole.
Shut-off surface patch tangent to the walls of the hole.

Shut-off surface patch tangent to the surface that the hole penetrates.
 No-Fill. Does not create a surface (the through hole is not patched). This option informs
the SOLIDWORKS application to ignore these edges when determining if the core and the
cavity are separable.
To separate the tooling block into two pieces, you need two complete surfaces (a core
surface and a cavity surface) without any through holes. Ideally, the Shut-off Surfaces
tool automatically identifies and fills all the through holes. Occasionally, the software
cannot generate a surface for a particular through hole. In that case, you need to identify
the through hole by selecting a loop of edges and selecting the No Fill option. After you
close the Shut-Off Surfaces PropertyManager, you create the surface patch manually. The
following SOLIDWORKS tools and capabilities are useful when patching through holes
manually:
o Tools on the Surfaces toolbar
o Smart Selection in lofts and sweeps
o The ability to create planar surfaces between any two planar edges
3. Click Zoom In/Out (View toolbar) and enlarge the image.
4. Click .

The uneven coloring of the model occurs because the cavity surface is coincident with the
faces of the solid body.
A Closer Look At Cavity, Core, and Shut-
off Surfaces
When you created the parting line, the software defined two surfaces:
Surface Duplicates these faces of the model Default color
cavity top green
core bottom red
In the Shut-Off Surfaces PropertyManager, you created surfaces to patch each through
hole, which were knitted into the cavity and core surfaces.
The surfaces are listed in Cavity Surface Bodies and Core Surface Bodies ,
under Surface Bodies in the FeatureManager design tree.
Cavity surface

Part
Core surface
XI. Creating Parting Surfaces
Parting surfaces extrude from the parting line and are used to separate the mold cavity
from the core.
1. Click Parting Surfaces (Mold Tools toolbar).
2. In the PropertyManager, under Mold Parameters, select Perpendicular to pull.
3. Under Parting Surface, set Distance to 10.
4. Under Options, select Knit all surfaces and Show preview.
5. Click .
The parting surface appears in Parting Surface Bodies , which is under Surfaces
Bodies in the FeatureManager design tree.
XII. Preparing for the Tooling Split
Create a parting plane that is perpendicular to the pull direction.

1. Click Rotate View (View toolbar) and turn the model to view the bottom side with
negative draft.
2. Click Zoom to Area (View toolbar) and zoom in to the rectangular rib above the
mouthpiece.
3. Select the top face of the rib.

4. Click Zoom to Area (View toolbar) to close the tool.
5. Click Plane (Reference Geometry toolbar).
6. Click Front (Standard Views toolbar).
7. In the PropertyManager, under First Reference, Face<1> appears in First Reference
:
a. Click Offset distance and enter 20.
b. If necessary, select Flip offset to position the plane below the reference face.
8. Click .
XIII. Applying the Tooling Split
Next, sketch a rectangle on the plane to create a planar surface.
1. Click Draft Analysis (Mold Tools toolbar) to turn off the draft analysis results.
Close the PropertyManager if it appears.
2. Click Tooling Split (Mold Tools toolbar).
A sketch opens.
3. Select Plane10 in the FeatureManager design tree.
4. Click Normal to (Standard Views toolbar).
5. Click Hidden Lines Removed (View toolbar).
6. Click Corner Rectangle (Sketch toolbar), sketch a rectangle, and dimension as
shown.
The vertical dimension (85) is from the endpoint of the arc to the bottom edge of the
rectangle. The horizontal dimension (175) is from the origin to the left edge of the
rectangle.

7. Exit the sketch.
XIV. Completing the Tooling Split
In the PropertyManager, the following appears:
 Shut-Off Surface1[1] under Core
 Shut-Off Surface1[2] under Cavity
 Parting Surface1 under Parting Surface
2. Under Block Size:
a. Set Depth in Direction 1 to 90.
b. Set Depth in Direction 2 to 70.
c. Select Interlock surface.
About Interlock Surfaces
The interlock surface surrounds the perimeter of the parting surfaces in a nearly
perpendicular direction at (in most instances) a 5° taper. As with all drafted faces, the
interlock surface drafts away from the parting line. Interlock surfaces are used to:
 Seal the mold properly to prevent liquids from leaking.
 Guide the tooling into place during the molding process.
 Maintain alignment between the tooling entities.
 Prevent shifts, uneven surfaces or incorrect wall thicknesses.
 Minimize the cost of machining the mold plates across the split, because the area
surrounding the interlock is planar.

d. Set Draft Angle to 3.
3. Click Wireframe (View toolbar).
4. Click to create the core and cavity blocks.

You can also create side core features if the model includes undercut areas (trapped areas
that prevent the part from ejecting from the mold).
Adding a Side Core
The Core tool extracts geometry from a tooling solid to create a core feature.
For example, suppose the telephone handset has a hole in its side for a cord clip. The
faces of the hole are undercut faces (trapped areas that would prevent the part from
ejecting from the mold). You need to create a side core. When the main core and cavity
are separated, the side core slides in a direction perpendicular to the motion of the main
core and cavity, enabling the part to be ejected.
To create a core:
1. Create a core sketch on or near the inside face of a tooling body. In this case, the sketch
was created on a plane parallel to the end face of the cavity body and through the
outermost point on the part.

The angled sides in the core sketch provide draft for the vertical movement of the cavity.
The draft angle specified in the PropertyManager provides draft for the horizontal
movement of the side core.
2. Click Core (Mold Tools toolbar).
3. In the PropertyManager set options such as Extraction direction, Draft Angle, End
Condition, and Cap ends, then click .
A new body is created for the core and is subtracted from the cavity body. In the
FeatureManager design tree, in Solid Bodies , the new core appears in Core bodies
.
You can also use the Core tool to create inserts, lifters, and trimmed ejector pins.

XV. Moving the Core from the Cavity
Use the Move/Copy Bodies feature to separate the core from the cavity.
2. Click Move/Copy Bodies (Features toolbar).
In the PropertyManager, click Translate/Rotate if you do not see the Translate group
box.
3. In the graphics area, select the cavity body.
The cavity is highlighted, and Tooling Split1[2] appears for Solid and Surface or
Graphic Bodies to Move/Copy in the PropertyManager.

4. Clear Copy.
5. Under Translate, set Delta Y to 160.
6. Click .
XVI. Displaying the Core and Cavity
Entities

Now display the core and cavity entities without additional bodies or surfaces.
1. To hide the solid body of the phone: Under Solid Bodies(3) , right-click Parting Line1
and select Hide .
2. To hide the cavity, core, and parting surfaces: Under Surface Bodies(4) , right-click
each of the following folders and select Hide :
o Cavity Surface Bodies(1)
o Core Surface Bodies(1)
o Parting Surface Bodies(1)
XVII.Enhancing Mold Visibility
Use the Appearances PropertyManager to change the colors and to apply transparency
to the core and cavity.
1. Near the bottom of the FeatureManager design tree, click Tooling Split1 > Appearances
> Tooling Split1.
2. In the PropertyManager, under Color, select (orange) from the swatch.
3. Click Advanced and select the Illumination tab.
4. Move the Transparent amount slider approximately halfway to adjust the cavity
transparency.

5. Click .
6. Save the part.
XVIII. Renaming and Saving the
Tooling Bodies
You now have a multibody part file, which maintains your design intent in one convenient
location. Changes to the telephone handset model are automatically reflected in the
tooling bodies.
Now create an assembly where you can add other supporting hardware, create assembly
features, and so on. First, rename the tooling bodies for easier identification. Next, save
the bodies in separate part documents.
1. In the FeatureManager design tree, in Solid Bodies , click-pause-click Tooling
Split1[1].
The body name is highlighted and ready to rename.
2. Type Core and press Enter.
3. Repeat steps 1 and 2 for Body-Move/Copy1, and name it Cavity.
4. In the FeatureManager design tree, in Solid Bodies , right-click Core and select
Insert into New Part.
If a dialog appears asking if you want to change the unit of measure in the derived part,
click Yes.
5. Enter MyTelephone-Core.sldprt and click Save.
If the Insert Into New Part PropertyManager appears, for File Name, click Browse (...),
name the new part, click Save and click .
6. Click Save All if the software prompts you to save component documents.

7. Click Window and select MyTelephone.sldprt to return to the telephone handset part.
8. In the FeatureManager design tree, in Solid Bodies , right-click Cavity and select
Insert into New Part.
9. Enter MyTelephone-Cavity.sldprt and click Save.
If the Insert Into New Part PropertyManager appears, for File Name, click Browse (...),
name the new part, click Save and click .
Click Save All if the software prompts you to save component documents.
XIX. Creating the Tooling Assembly
Now create an assembly containing the tooling parts.
1. Create a new assembly document.
2. In the Begin Assembly PropertyManager, click .
3. Under Part/Assembly to Insert, select MyTelephone-Core and drop it in the graphics
area.
4. Repeat step 3 for MyTelephone-Cavity.
5. Click to close the PropertyManager.
The two tooling parts are now components of the assembly, with external references to
MyTelephone.sldprt. You can add other supporting hardware, create mates, and so on.
Changes to the telephone handset model are automatically reflected in the tooling parts
in the assembly.

Congratulations! You have completed this tutorial.

Molds design in solid works

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