Defining End Cuts based on a User Defined Feature

This task shows you how to build an end cut based on a User Defined Feature (UDF). This is usually done by an administrator.

Most of these steps apply to the Structure Functional Design, Ship Structure Detail Design, and Structure Design applications. Certain steps, where indicated, apply to just one or two of the applications.

An end cut is a closed surface or a volume that will be subtracted from the profile (shape/stiffener). This closed surface (or volume) is modeled using a user defined feature (UDF). Both the Wireframe and Surface Design and Generative Shape Design workbenches can be used to create the end cut geometry.
 
A PKT license is required to build the user defined features.

A GSO license is required if volumes are used to define the end cut geometry.

Starter models are provided to help in the creation of new end cuts. These templates are located in the following folder:

../OS/startup/EquipmentAndSystems/Structure/DetailingFeatures/UDFTemplates

For more information and additional guidelines for defining geometry, see Defining Support Geometry.
  The following explains how to create a basic snipe radius end cut.
1. Open the starter CATPart and save it as a new CATPart.

For organizational purposes, it is recommended that you create all the features used to design the end cut geometry under a geometrical set called UDF Definition.
 
2. Using the Point command, create a point at the middle of the curve called Shape_Edge_Start_MoldedFlange1.

 
3. Using the Plane command, create a plane normal to the curve at the new point.

 
4. Using the Circle command, create a 50 mm circle with the point as origin and the plane as support.

 
5. In the Generative Shape Design workbench (Start - Shape - Generative Shape Design), select the Volume Extrude command (Insert - Volumes - Toolbar).

Select the circle as profile and the plane as direction.
  If you don't have access to the Volumes toolbar (because you don't have a GSO license), you must create a closed surface.
Create a surface from the circle using the Fill command.
Extrude this surface using the Extrude command.

The result is a closed surface that can be used to define an end cut.
 

Naming Conventions for Section Characteristics

When you define your end cut UDF, follow these naming conventions:
 
Inputs corresponding to the profile to be cut (shape/stiffener) have no index in their names. For example:
Shape_Face_MoldedFlange1
Shape_Edge_Start_MoldedFlange2
 
For a standard end cut (non-contextual):
  • If an end cut definition requires geometries from both extremities (For example, Shape_Face_Start and Shape_Face_End), then the end cut geometry has to be designed at the Start extremity of the shape or stiffener.

For a contextual end cut:

  •  Inputs corresponding to the context have an index in their names. For example:
Shape1_Face_MoldedFlange1
Shape1_Edge_Start_MoldedFlange2
  • The end cut definition must use both extremities (For example, Shape_Face_Start and Shape_Face_End) of the profile to be cut. Then, a Knowledgeware Rule (comparing the distance between Shape_Face_Start and the context with the distance between Shape_Face_End and the context) must be used to determine on which extremity the end cut will be applied. 
  • Refer to the sample end cut template, _Template_for_ContextualPlateEndcut_Tees.CATPart. It is located in the following folder:

       ..OS/startup/EquipmentAndSystems/Structure/DetailingFeatures/UDFTemplates

For more information on naming conventions, see Defining Support Geometry.

Creating the End Cut UDF
 
6. Select Insert - UserFeature - UserFeature Creation... from the menu bar to define the end cut UDF.

The Userfeature Definition dialog box opens.

Give the end cut UDF a meaningful name. This is the name the user will see when he instantiates the end cut in his design.

Select UDF Definition in the specifications tree.

Select the Inputs tab on the Userfeature Definition dialog box.

If the starter model has been used, all the inputs should follow the naming convention.

As shown above, our UDF has only one input: an edge named Shape_Edge_Start_MoldedFlange1.
 

  
  7. Select the Parameters tab. Publish the Radius parameter corresponding to the circle created previously by double-clicking it.

NOTE: Only published parameters will be accessible when using this end cut.
 
  8. Select the Outputs tab. Main Result is the Volume Extrude feature (or the closed surface). It must display in the Output Name column. If Main Result does not display, select Add, Remove or Replace, and ensure that it does display.

Click OK when done.
 
The end cut UDF is created under the Knowledge Templates entry in the specifications tree.

 

  
9. Store the end cut UDF in the detailing features catalog. For more information, see Adding Slots, End Cuts and Small Assemblies Templates to a Catalog.
 

Creating the Catalog Selection Preview Image
 
  When placing the end cut in the Structure Design application, a preview of this end cut displays in the Catalog Selection for End Cut dialog box.

Follow these steps to create a preview image that is representative of the actual end cut.

Use the Part Design workbench and select the Pocket command.

Create a Pocket in the PartBody by selecting the circle. Apply the standard isometric view to your document. Place all 3-D construction geometry in No-Show, then save the document.

It should look like this:

In the Structure Design application, when you place this end cut, the preview in the Catalog Selection for End Cut dialog box looks like this: