Model a New Assembly Machining Tool

A tool for machining assembly parts or sheet-metal parts is modeled like a normal part. Machining features are modeled by defining the extrusion based on a sketch as a tool in the feature properties. If the extrusion based on a sketch has not been defined as a tool, the geometry will not have a machining effect.

Model a new assembly machining tool as follows:

  1. Begin a new part model by selecting >  New and selecting Part.
  2. Sketch and model the part's geometry that will not have a machining effect.
    Note: The origin of the part's first sketch will become the handle of the finished tool when you save the part. If this point is not suitable for the tool's handle, you can define a new handle after the part is finished but before saving the part.
  3. Model the machining feature. Define a boss feature as a tool by selecting Make Tool in the feature properties. A feature defined as a tool will remove material when the tool is added to an assembly.
  4. If necessary, edit the machining feature with a bevel or rounding, for example.
  5. Sketch and add other machining or regular features, if necessary. Regular features will add material, when the tool is added to an assembly.
  6. If necessary, add a dimension table for the tool. With a dimension table you can edit the tool’s dimensions when you add it to an assembly. Create a Dimension Table (3D)
  7. If necessary, move the tool’s handle. Move a Handle
  8. If necessary, prevent the tool from showing in an assembly parts list and/or drawing. Select the context-sensitive function Properties and unselect To Assembly Parts List and/or To Assembly Drawing.
  9. When the tool is finished, save it either as a regular part to the archive or as a component to the component library. Save the tool as a component by selecting the context-sensitive function Save To Library > As Component....
  10. Select the tool's execution order in the Choose tool execution order dialog box. If you select Tool geometry first, the tool will remove material first and then add material. If you select Additive geometry first, the tool does the opposite. If you select Tool geometry stays as tool geometry, the tool geometry will remain in the tool when it is added to an assembly.
  11. Select OK.
  12. Select the folder to which you wish to save the tool, and name the file. If necessary, create a new folder.
  13. Select Save.