Creating Slots

In this section, you will also find the following reference information:

• How to Define a Slot
• Profiles
• Center Curves
• Profile Control

1. Click Slot .
   The Slot Definition dialog box is displayed.

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

3. Click to open the Sketcher and edit the profile. This temporarily closes the dialog box.

4. For example, enlarge the profile.

5. Quit the Sketcher when done.
   The Slot Definition dialog box reappears.

6. 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. The application previews the slot.

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.
   Merge slot's ends is to be used in specific cases. It creates material between the ends of the slot and existing material. For an example, refer to Trimming Ribs or Slots.

9. To add material equally to both sides of the profile, check 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.

How to Define a Slot

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

	Closed Profile	Open Profile
Open Center Curve		(Thick Profile Option)
Closed Planar Center Curve
Closed 3D Center Curve		(Thick Profile Option)

Profiles

When selecting a profile, keep in mind that:

• You can use wireframe geometry as your profile.

• It is recommended that the profile be on the center curve in a plane normal to the center curve. Otherwise, it may lead to an unpredictable shape.

• 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.

• You can also create a profile by using any of these creation contextual commands available from the Profile field:

  • Create Sketch: launches the Sketcher after selecting any plane, and lets you sketch the profile you need as explained in the Sketcher User's Guide.

  • Create Join:  joins surfaces or curves. See Joining Surfaces or Curves.

  • Create Extract:  generates separate elements from non-connex sub-elements. See Extracting Geometry.
    If you create any of these elements, the application then displays the corresponding icon in front of the Selection field. Clicking this icon enables you to edit the element.
    If you have chosen to work in a hybrid design environment, the elements created on the fly via the contextual commands mentioned above are aggregated into sketch-based features.

• You can use an open profile provided existing material can trim the slot. For more information, refer to Trimming Ribs or Slots.

Center Curves

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.
• center curves must not be composed of several geometric elements

Profile Control

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.

• Contextual commands creating the directions you need are available from the Selection field:
  • Create Line: For more information, see Creating Lines
  • Create Plane: see Creating Planes
  • X Axis: the X axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Y Axis: the Y axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Z Axis: the Z axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Create Join: joins surfaces or curves. See Joining Surfaces or Curves.
  • Create Extrapol: extrapolates surface boundaries or curves. See Extrapolating Surfaces and Extrapolating Curves.
    If you create any of these elements, the application then displays the corresponding icon in front of the Selection field. Clicking this icon enables you to edit the element.
    If you have chosen to work in a hybrid design environment, the elements created on the fly via the contextual commands mentioned above are aggregated into sketch-based features.
•  Move profile to path: easily associates profiles with center curves but also sweeps a single sketch along multiple center curves.
  This option can be accessed if Pulling direction of Reference surface is already on, and builds the profile with the following understanding:
  • The origin of the sketch plane (i.e. 0,0) will be swept along the path.
  • The vertical axis of the sketch plane (i.e. 0,1) will be kept parallel to either the pulling direction (if the profile control is set to Pulling direction) or the normal to the Reference surface (if profile control is set to Reference surface).