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

To define a slot, you need a center curve, a planar profile, a reference element and optionally a pulling direction. 

To create slots you can combine the different elements as follows:

Open profile Closed profile Pulling direction
Open center curve

Closed planar center curve  
Closed 3D center curve    

Moreover, the following rules should be kept in mind:
3D center curves must be continuous in tangency.
if the center curve is planar, it can be discontinuous in tangency.

Open the Slot1.CATPart document.
1.  Click the Slot icon .

The Slot Definition dialog box is displayed.



Select the profile, i.e. Sketch.2.

The profile has been designed in a plane normal to the plane used to define the center curve. It is closed.


About Profiles

You can use wireframe geometry as your profile too.
In some cases, you need to define whether you need the whole sketch, or sub-elements only. For more information, refer to Using the Sub-elements of a Sketch.
Slots can also be created from sketches including several profiles. These profiles must be closed and must not intersect. 
If you launch the Slot command with no profile previously defined, just click the icon to access the Sketcher and then sketch the profile you need.
  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.

You can control the profile position by choosing one of the following options:

Keep angle: keeps the angle value between the sketch plane used for the profile and the tangent of the center curve.
Pulling direction: sweeps the profile with respect to a specified direction.

For example, you need to use this option if your center curve is a helix. In this case, you will select the helix axis as the pulling direction. 

Reference surface: the angle value between axis h and the reference surface is constant.

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 rib you can use open profiles and closed center curves too. Center curves can be discontinuous in tangency.

The application previews the slot.

  Clicking the icon opens the Sketcher to let you edit the center curve. 
The Merge ends option is to be used in specific cases. It lets the application create material between the ends of the slot and existing material.
  7.  Check the Thick Profile option  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.

  Checking the "Merge Ends" option trims the rib to exiting material.
  9. To add material equally to both sides of the profile, check "Neutral fiber" and preview the result.

The thickness you defined for Thickness1 (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.


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