Select File > New
Select Part in the list.
Using the contextual menu, edit the part properties,
go to the Product tab and type MoldedPart as its
(You can also begin by creating a mold base
an empty MoldedPart where you can complete the steps given
Tel.CATPart file in the Samples directory. This opens a new viewer.
Select the PartBody in the
specifications tree and copy it.
Select the Part in the
MoldedPart viewer and use the Paste special function in
the contextual menu.
Select AsResultWithLink in the
dialog box and click OK.
This ensures that if the original part to mold is modified that the
modifications will be applied to the MoldedPart.
You can now
perform a scaling operation to take account of shrinkage:
- Select Start > Mechanical Design > Part Design.
- Right-click Body.2 in the specifications tree and
select Define In Work Object in the contextual menu.
- Click Scaling
- Type a ratio value of 1.03 (for example), select the xy plane in
the tree as reference and click OK.
Repeat this action for the yz and zx planes with
different ratio values.
determine the pulling direction with Draft Analysis or the
Core and Cavity Design workbench:
the main pulling direction is defined when the CavitySurface and the
CoreSurface are separated.
From the Core and Cavity Design workbench, you obtain surface
joins for the CavitySurface and the CoreSurface.
An axis system is also created and used for the definition of the main
Hide Core.1, Cavity.1, Other.1
Select Start > Shape > Generative Shape Design.
Insert an Geometrical set and name it PartingBody.
Select all of the bottom edges of the part. Click OK
in the dialog box to confirm the action.
Right-click the new join in the specifications tree to
open its properties and call it PartingLine.
Now you are going to fill the hole on the part to enable
the split of the CavityPlate and of the CorePlate.
Join the curves around the hole and click OK in the dialog box.
Select Join.2 in the specifications tree.
Click OK in the dialog box. The hole is filled.
thing you are going to do is to create the
- Click Sweep
- Click the Line Profile button in the dialog box.
- Select With reference surface for the Subtype.
- Select PartingLine in the specification tree for the
- Select xy plane in the specification for the Reference
- Type a value of 20 mm for Length 1.
- Click OK.
The parting surface is created
(if it is created in the wrong direction, i.e. in the inside of the part,
swap the values of Length 1 and Length 2).
Using the contextual menu, change the sweep name to PartingSurface.
Since the PartingSurface is shared by both the
CavitySurface and the CoreSurface,
it is generated on
Select Tangent continuity in the Propagation type
pick any face on the upper surface in the viewer for the To
Turn the part over and repeat this step for the underside
Select PartingSurface, the fill and the first extract in the
Clear the Check connexity check box.
the new join in the tree.
Select Properties in the contextual menu and change the name to
Repeat the action with the parting surface, fill and the
Call the new join
Your specification tree should look like this: