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.

Related Topics
More about Slots
Trimming Ribs or Slots
Using the Sub-Elements of a Sketch
Creating Thin Solids

  1. Click Slot .

    The Slot Definition 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. For example, enlarge it.

  5. Quit the Sketcher.

    The Slot Definition dialog box reappears.

  6. To go on with our scenario, let's maintain the Keep angle option. Now, select the center curve along which the application 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 application previews the slot.



    Important: Clicking the icon opens the Sketcher to let you edit the center curve.

  7. Select Thick Profile to add thickness to both sides of Sketch.2.

    New options are then available:

  8. 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. For an example, see Trimming Ribs or Slots.

  9. To add material equally to both sides of the profile, select Neutral fiber and preview the result.

    The thickness you defined forThickness1 (2mm) is now evenly distributed: a thickness of 1mm has been added to each side of the profile.

  10. Click OK.

    The slot is created. The specification tree indicates this creation.