Interactive Templates Quick Reference

User Features

Creating a User Feature
Saving a User Feature in a Catalog
Instantiating a User Feature from a Catalog
Instantiating a User Feature from a Document
Instantiating a User Feature from a Selection
Editing a User Feature
Managing the orientation of the items making up the User Feature (planes, curves, ...)
after instantiating the User Feature in Edit mode
Working with the User Feature Definition Window

1. Open a .CATPart file.

2. Select Insert>UserFeature>UserFeature Creation... from the standard menu bar or click the Create a UserFeature icon (). The User Feature Definition dialog box is displayed. 

3. Replace the default User Feature name, then select the object in the specification tree.

4. Select the Outputs tab. Specify the main result.

5. Click OK in the dialog box. The User Feature is added to the specification tree.

1. Open a .CATPart file.

2. Click the Save in Catalog icon () from the standard menu bar. The 'Catalog save' dialog box is displayed.

3. Select the Create a new catalog option and click the button on the right-hand side of the Catalog name field. The dialog box displayed allows you to create a .catalog file where to store the created User Features. Enter a file name and click Open. Then click OK in the Catalog save dialog box. The catalog containing the User Feature is created.

1. Open a .CATPart file.

2. In the standard toolbar, click the Open Catalog icon. The catalog browser is displayed.

3. Click the icon. In the dialog box which is displayed, select the catalog which contains the User Features that you want to instantiate. Click Open to open the selected catalog. The dialog box which is displayed next depends on your last interaction on this catalog. Double-click the object displayed in the left pane until the User Feature is available.

4. To instantiate the object into the document:

   1. If need be, select the feature in the Insert Object dialog box, then select the feature in the document geometry area or in the specification tree.

   2. Click Parameters. The dialog box which is displayed provides you with the way to modify the parameter you have declared as published at the User Feature creation. Modify the value (if necessary).

   3. Click OK to instantiate the User Feature and exit the Insert Object dialog box. The User Feature is instantiated into the document. 

1. Open a .CATPart file.

2. Click the Instantiate an element stored in a document icon. The File Selection dialog box is displayed.

3. Select the .CATPart file containing the User Feature to instantiate, and click Open. The Insert Object dialog box is displayed.

4. To instantiate the object into the document:

   1. If need be, select the feature in the Insert Object dialog box, then select the feature in the document geometry area or in the specification tree.

   2. Click Parameters. The dialog box which is displayed provides you with the way to modify the parameter you have declared as published (if any) at the User Feature creation. Modify the value (if necessary).

   3. Click OK to instantiate the User Feature and exit the Insert Object dialog box. The User Feature is instantiated into the document. 

1. Open the CATPart file that will contain the User Feature instance as well as the file containing the User Feature that you want to instantiate.

2. Tile the window vertically.

3. Expand the KnowledgeTemplates node in the file containing the User Feature and click the User Feature once.

4. Go to the file that will contain the User Feature and click the Instantiate from Selection icon (). The Insert Object dialog box is displayed.

5. Make the appropriate selections and click OK to instantiate the User Feature and exit the Insert Object dialog box. The User Feature is instantiated into the document. 

1. Open the PktManagingPlanes.CATPart file.

2. From the Standard menu, select Insert>Instantiate from Document... .

3. In the File Selection window, select the PktPlaneUDF.CATPart file and click Open.

4. The Insert Object dialog box is displayed. Select:

   	Plane.1=zx plane
   	Point.1=Point.1
   	Plane.2=xy plane

5. Reverse the direction of Plane.1 and Plane.2 and click OK when done. The User Feature is instantiated.

6. Double-click UDF.1 in the specification tree. The Definition box of the User Feature is displayed.
   Note that even if the selected inputs are both planes, in the first case (Plane.1), the display shows the zx plane as selected, and in the second case (Plane.2), the display shows a new element (Inverse.1) which was created and inserted at instantiation. Click OK to exit the dialog box.

7. Open the PktPlaneUDF.CATPart file and double-click the User Feature:

   	The input corresponding to Plane.1 is pointed by a Sketch: The orientation of Plane.1 is performed inside the Sketch feature. That is why the input is still the zx plane.
   	The input corresponding to Plane.2 is pointed by a surfacic feature (Extremum.1): To manage the orientation of surfacic features, an Inverse feature is created. That is why the input references Inverse.1.

8. Go back to the PktManagingPlanes.CATPart file and double-click the UDF1.1.

9. Select Plane.1 in the Definition box.

   Note that the orientation of the zx plane is not identical to the one you selected at instantiation. It is a default orientation for the input. If you click the corresponding arrow, you can modify this orientation to get the desired one.

10. Select Plane.2 in the Definition box.

    Note that the orientation is the default one for the Inverse.1 feature. If you click the corresponding arrow in the geometry, you can modify the orientation of the User Feature input. You will see then that the Inverse feature disappears or reappears depending on the direction of the arrow.

1. Open the PktModifyingMainResult.CATPart file.

2. Double-click UserFeature1 located below the KnowledgeTemplates node. The User Feature Definition window is displayed.

3. Click the Outputs tab. 

   Suppose you are only interested in instantiating the CloseSurface object of Assemble.2.
   	Select the Main result output.
   	Click Replace, then select the CloseSurface.2 feature in the specification tree. The  CloseSurface.2 feature will be the only object carried forward to the receiving document during the instantiation process (no supporting pad).
   Suppose you want to instantiate the Assemble.2 feature as a whole plus one of the circles required to build the Body.2 object (Circle.2 for example).
   	Specify Assemble.2 as a main result
   	click Add, then select the Circle.2 object in the specification tree. The instantiation process will carry  forward the Assemble.2 object and the Circle.2 object to the receiving document.
   	Note that the dimension of the secondary outputs must always be inferior to the Main result.

1. Open a .CATPart file.

2. Select Insert>Userfeature>Userfeature Creation... from the standard menu bar. 

3. In the Definition tab, replace the default User Feature name (enter Pad1 as a new name for example) then select a feature in the specification tree.

4. In the Type tab, enter the name of the instance type: Enter the first part of the type in the first box, the second part in the second box and press Enter.

5. Click Manage Type. Indicate the Super Type and the Package.

6. Click Create Type, Save, Close.

Power Copies

Creating a Power Copy
Saving a Power Copy in a Catalog
Instantiating a Power Copy from a Catalog
Instantiating a Power Copy from a Document
Instantiating a Power Copy from a Selection
Editing a Power Copy
Introducing the Power Copy Definition Window

1. Open a .CATPart file

2. Select Insert >Advanced Replication Tools > PowerCopy Creation...or click the Create a PowerCopy icon ().

3. Select the elements making up the Power Copy from the specification tree.

4. Define the Power Copy as you want to create it.

5. Click OK to create the Power Copy.

1. Open a .CATPart file containing a Power Copy. The Power Copy is displayed below the Power Copy node.

2. Click the Save in Catalog icon () from the standard menu bar in the PKT workbench. The 'Catalog save' dialog box is displayed.

3. Select the Create a new catalog option and click the button on the right-hand side of the Catalog name field. The dialog box which is displayed allows you to specify a .catalog file where to store the created Power Copies. Enter a file name and click Open. Then click OK in the Catalog save dialog box.

1. Open the .CATPart file that will contain the instantiated Power Copy.

2. In the standard toolbar, click the Open Catalog icon. The catalog browser is displayed.

3. Click the icon. In the dialog box which is displayed, select the catalog which contains the Power Copy that you want to instantiate. Click Open to open the selected catalog.

4. Double-click the object displayed in the left pane until you get the object to be instantiated.

5. Double-click the object. The Insert Object dialog box is displayed.

6. If need be, select the feature in the Insert Object dialog box, then select the feature in the document geometry area or in the specification tree.

7. Click OK to instantiate the Power Copy and exit the Insert Object dialog box. The Power Copy is instantiated into the document. 

1. Open a .CATPart file.

2. Click the Instantiate an element stored in a document icon () . The File Selection dialog box is displayed.

3. Select the .CATPart file containing the Power Copy to instantiate, and click Open. The Insert Object dialog box is displayed.

4. To instantiate the object into the document:

   1. If need be, select the feature in the Insert Object dialog box, then select the feature in the document geometry area or in the specification tree.

   2. Click Parameters. The dialog box which is displayed provides you with the way to modify the parameter you have declared as published (if any) at the Power Copy creation. Modify the value (if necessary).

   3. Click OK to instantiate the Power Copy and exit the Insert Object dialog box. The Power Copy is instantiated into the document. 

1. Open the .CATPart file that will contain the Power Copy as well as the file containing the Power Copy that you want to instantiate.

2. Tile the window vertically.

3. Expand the Power Copy node in the file containing the Power Copy and click the Power Copy once.

4. Go to the file that will contain the Power Copy and click the Instantiate from Selection icon (). The Insert Object dialog box is displayed.

5. Make the appropriate selections and click OK to instantiate the Power Copy and exit the Insert Object dialog box. The Power Copy is instantiated into the document. 

Part and Assembly Templates

1. Open a .CATPart file.

2. From the Insert menu, select Document Template Creation ... or click the Create a Document Template icon ().

3. In the Document Template Definition window, click the Inputs tab and select the inputs you want to select.

4. In the Document Template Definition window, click the Published Parameters tab to publish parameters (if need be.)

5. Save the file (note that you can save the document template in a catalog.)

1. Open a .CATProduct file.

2. Click the Catalog icon and select the catalog you created when creating the template.

3. Double-click the family and the Document Template.1 template.

4. In the Insert Object window, click Use Identical Name in the Insert Object window. Make the appropriate selections in the viewer when necessary and click OK when done.