Creating Slots

You can sweep a profile along a center curve to remove material for creating a slot. To define a slot, you need a center curve, a planar profile, a reference element and optionally a pulling direction.

This task shows you how to create a slot, that is how to sweep a profile along a center curve to remove material.

Before you begin:

Make sure that the Open dialog boxes with legacy appearance check box available at Me > Preferences > App Preferences > 3D Modeling > 3D Modeling Core > Part Design > Appearance of dialog boxes, is selected.

See Also
About Slots
About Trimming Ribs or Slots
  1. From the Model section of the action bar, click Slot .
    The Slot.x dialog box appears.
  2. Select the profile.
    The profile has been designed in a plane normal to the plane used to define the center curve. It is closed.

  3. Click the icon to open the Sketcher .
    This temporarily closes the dialog box.
  4. Edit the profile and quit Sketcher.
    The Slot.x dialog box reappears.
  5. To go on with our scenario, let's maintain the Keep angle option. Now, select the center curve along which the app will sweep the profile. The center curve is open. To create a slot you can use open profiles and closed center curves too. Center curves can be discontinuous in tangency. The app previews the slot.


    Important: Clicking the icon opens the Sketcher to let you edit the center curve.
  6. Click to add thickness to both sides of the sketch.
    New options are then available.
  7. Enter 2mm as Thickness1 's value, and 5mm as Thickness2 's value, then preview the result.
    Material is added to each side of the profile.

    Selecting Merge Ends trims the slot to existing material.

  8. To add material equally to both sides of the profile, select Neutral fiber and preview the result.
    The thickness you defined forThickness1 is now evenly distributed: a thickness of 1mm has been added to each side of the profile.

  9. Click OK.
    The slot is created. The tree indicates this creation.