Model a New Machining Feature

General

Machining geometry is created in two ways:
  • When you perform the operation Boss Extrude for a sketch, select the option Make Tool.
  • Model the part, and select Properties and Tool, so that the geometry of the part will be a tool in its entirety.
  • The machining geometry is drawn in red color.
  • Note that the thread part of the machining thread feature is drawn like a normal thread.

Steps when a part has regular geometry and a machining feature.

  1. Start a new part model
    • File > New.
    • Select Part.
    • Enter the archive data
  2. Sketch the geometry of the part and perform the necessary boss and cutout extrusions and other features.
    • Note that the origin point of the first sketch of the part acts as a locating point.
    • However, it is worth adding a grip to a library feature. Add a Grip Point
  3. Sketch the machining feature's geometry.
    • If you are only modeling a machining feature without boss geometry, first model the part as finished, and then change its properties to a tool (see the General section).
  4. Accept the sketch.
    • From the ribbon bar with the function Sketch | Return | OK or
    • Select the context-sensitive function OK.
  5. Perform the operation Boss Extrude for the sketch and select the option Tool.
  6. If necessary, edit the machining feature with a bevel or rounding, for example.
  7. If necessary, add a dimension table for the model.
    • With a dimension table, you can control both the regular geometry and the geometry of the machining tool.
    • For more details, see Edit the Dimension Table of a Part Model
    • When creating a sheet metal machining feature, enter the letter t in the Formula field of the feature to have the sheet thickness always automatically checked from the model.
  8. If you create a sheet machining feature, change Sheet Metal as the part's type by selecting the context-sensitive function Properties and selecting Sheet Metal in the Type section.
  9. When the part model is finished, save it by selecting the context-sensitive function Save To Library > As Feature.
  10. Select the machining feature's execution order in the Choose tool execution order dialog box.
    • Select Tool geometry first if you want the machining feature to remove the material first and then add the feature geometry.
    • Select Additive geometry first if you want to add the geometry of the feature first and then remove the machining feature from the part.
    • Select Tool geometry stays as tool geometry if you want the feature tool to remain a tool when it is added to a part model.
  11. Select OK.
  12. Select the folder to which you wish to save the feature, and name the file. If necessary, create a new folder.
  13. Select Save.