Creating a Punch with a Die

First, you will define a punch and a die in Part Design, in the absolute axis-system.
Then, in a Sheet Metal part, you will bring the punch and the die features (and their axis system) to a point you have selected. If necessary, you will define a rotation of the axis system from a reference line.

This user-defined stamping cannot be combined with the Opening and Cutting Faces approach.

Creating Stamps

1. Start the Part Design workbench.

2. Insert a body (menu Insert  >  Body) to define the punch.

3. Enter the sketcher select the yz plane, and draw the profile of the punch, and a rotation shaft.

   The punch must be oriented as described in Defining the Punch in Relation to the base feature to be Stamped in the Creating User-Defined Stamping Features chapter.

4. Return to the 3D space and create the punch using Shaft .

5. Repeat from step 2 to step 4 to define the die, making sure that it is oriented as described in Defining the Die in Relation to the base feature to be Stamped in the Creating User-Defined Stamping Features chapter.

6. Return to the Sheet Metal application, and if needed, use the Define In Work Object on the PartBody containing the wall or the base feature to be stamped.

7. Click User Stamp in the Cutting/Stamping toolbar (Stamping sub-toolbar). The User-Defined Stamp Definition dialog box is displayed.

8. Select a base feature, or a face where the stamping is to be created. 
   This base feature or face is used to define the stamping location and direction, by matching the punch's origin to the selected point on the base feature.

9. In the Type list, select Punch and Die. The User-Defined Stamp Definition dialog box is updated as shown below:

   You can select the BothSides check box to stamp in two opposite directions of the stamping face in a single operation. In this case, the Faces for opening box is available. If you select the BothSides check box, the selected feature (punch or die) will not be split by the stamping face. In this case, the faces selected in the Faces for opening box is used to determine the portion of the selected feature to be removed. The icon to the right of the Faces for opening field lets you edit the list of opening faces.

10. In the Punch field, select the Punch feature from the specification tree.

    The punch's positioning is previewed in the geometry.

11. In the Die field, select the Die feature.

    The die's positioning is previewed in the geometry as well.

12. Select the No Fillet check box if you do not want the stamp to be filleted, or set the radius value if you want the stamp to be filleted.

    Stamp without fillet   Stamp with fillet

13. If needed, define the stamp's positioning on the selected base feature by choosing:

    a Reference for rotation: by default, it is the sketch axis, but you can also select any line or edge on base feature. a Rotation angle value: you can either enter a value in the dialog box, or use the manipulator in the geometry to define this value. a new Origin point on the base feature to coincide with the punch's point of origin. This is especially useful for non-circular stamps, but you can very well create the stamp as is, without further positioning.

    To edit the sketch having origin point, click Positioning Sketch . This option can be used only after selection of the origin point.

14. If needed, select the Position on Context check box (in the Generative Sheetmetal Design workbench only).
    The punch and die's positioning is previewed on the geometry.

    	When selecting the Position on Context check box, the stamp's positioning and direction are not defined in relation to the base feature anymore. Only the punch and die's axis system is taken into account and the stamp is created according to their positioning and direction.
    	Once Position on Context is selected, the position on wall cannot be modified nor the direction of the stamp: the fields available in Position on wall section and the Reverse direction button are disabled.

15. Click OK to validate and create the stamping.
    By default the Punch and Die parts are set in No Show mode when clicking OK to create the stamp on the base feature.

    	Radius is the radius of the bend between the stamping and the base feature. Punch and Die are the bodies you have defined previously. If the punch and the die are in another CATPart document, activate this document before clicking the punch or the die. If you select two reference lines in addition to the plane, this will create two editable constraints to position the stamping. These constraints are editable. A user-defined stamping can be edited (punch, die, position, constraints). As the punch and die are not symmetrical, you cannot create such features as a cutout, a hole, a corner, etc., on this kind of stamping.
    	If you enter a punch and a die, the stamping is the difference of the shape of both features. The punch height cannot be superior to the base feature height, otherwise it is considered as a cutout. You may create a user-defined stamping from a punch only but you cannot create a fillet.   Only the stamping sketch is displayed in unfolded views.
    	The punch and die bodies can be defined in the Sheet Metal part where the stamping is to be created (see PunchDie1.CATPart or NEWPunchDie1.CATPart in the samples directory). In this case, make sure you select the Define In Work Object on the PartBody containing the base feature to be stamped, prior to actually creating the stamp. or as two separate Part Design parts (Punch1.CATPart and Die1.CATPart from the samples directory) In this case, when selecting the punch or die feature, the system automatically copies this feature into the .CATPart document into which the base feature to be stamped is located. A link is retained between the initial punch or die feature and its copy.

Inserting Punch and Die Features from the Catalog
 

All .CATParts and catalog are available from the sample directory (Die.CATPart, Punch.CATPart, UserStamp_Catalog.catalog).

1. Select the face of the part where the stamping is to be created.

2. Click User Stamp to open the User-Defined Stamp Definition dialog box.

3. In the Type list, select Punch and Die. The User-Defined Stamp Definition dialog box is updated as shown below:
   
   

4. Click in the Punch box.
    

5. Click catalog to select a Punch feature from the catalog.
   The Catalog Browser dialog box is displayed.

6. Browse to the directory where UserStamp_Catalog.catalog is filed.
   
   

7. Double-click on chapter UserStamp.
   
   
   
   The parts saved in the catalog are displayed.
    

8. Select the Punch, then click on OK.
   
   
   
   The body of this punch is aggregated under the part in the specification tree. It is referenced in the User-defined Stamp Definition dialog box as Result of Punch in the Punch box.

9. Select the Die field to activate it.

10. Click catalog to select a Die feature from the catalog.
    The Catalog Browser dialog box is displayed.

11. Browse to the directory where UserStamp_Catalog.catalog is filed.

12. Double click on chapter UserStamp.

13. Select the Die, then click on OK.
    
    
    
    The body of this die is aggregated under the part in the specification tree. It is referenced in the User-defined Stamp Definition dialog box as Result of Die in the Die box.
    
    A punch and a die are now available for you to create a user-stamp.

14. Click on OK to create your stamp.

    	To insert a feature from the catalog, the appropriate field has to be selected first in the User-defined Stamp Definition dialog box. When creating a stamp from a catalog's feature, the Position on context option is deactivated. This is due to the fact that the stamping feature of the catalog was previously defined in its own axis-system. The part's canonic axis-system and the catalog's being different, there is no reason to use the option. Yet, when editing a user-stamp created from a catalog's features or using a body imported from another user-stamp, the option is activated. You can instantiate User Defined Features (UDFs) or power copies from a Sheetmetal catalog. For more information, refer to Browsing the SheetMetal Catalog.