Extruding

You can extrude open or planar profiles composed of lines, circles, curves, projection of lines, and projection of circles.

This task shows you how to:

Before you begin: Create a sketch representing a line or a planar profile.
See Also
About Extruding
Creating Rolled Walls

Create an Extrusion

You can create an extrusion.

  1. From the Model section of the action bar, click Extrusion .
  2. Select the sketch or the planar profile in the 3D area.
    It appears in the Profile box.
  3. Select the profile positioning option:
    OptionDescription
    Bottom Sets the sketch at the bottom position of the wall thickness.
    Middle Sets the sketch at the middle position of the wall thickness.
    Top Sets the sketch at the top position of the wall thickness.
  4. Optional: Select a fixed element in the Fixed Area box.
    It can be a border vertex or an edge of the profile.
  5. To define both limits, specify the limit type.
    OptionDescription
    Dimension Generates the extrusion using a length.
    Up to plane Generates the extrusion up to the defined plane.
    Up to surface Generates the extrusion up to the defined surface.
    Mid plane Generates the extrusion using a length that is equally divided between both limits of the extrusion. It is available only with Limit 1.

    If the limit is set to Dimension, you can click Mirrored Extent to extend the material on both sides of the sketch. In that case, only Limit 1 can be edited.

  6. Optional: To invert the direction of the extrusion, click Invert Direction .
  7. Optional: In the Bends frame, select With Bend.
  8. Optional: Select the unfold method, and specify its parameters:
    OptionDescription
    K-factorDefines the neutral fiber position inside the thickness, from the inner side of the bend.
    Bend AllowanceThe bend allowance corresponds to the unfolded bend width.
    Bend DeductionThe bend deduction represents the sheet metal deformation when the bend is unfolded.
    Bend Table from StandardsUses the bend deduction table defined in the standards. You must select a standard containing a bend deduction table.

    Note: The Bend Table from Standards unfold method is automatically selected if a bend table is defined in the Sheet Metal parameters. If you do not want to use this unfold method, you can choose another standard in the Sheet Metal parameters that does not contain a bend deduction table. For more information, see Editing the Sheet Metal Parameters.

  9. Optional: Select one of the following for each bend extremity:

    If you create a feature on the extruded profile, the bend extremities may be recomputed to ensure a consistent result.

    OptionDescription
    Minimum with no reliefThe bend corresponds to the common area of the supporting walls along the bend axis, and shows no relief.
    Square reliefThe bend corresponds to the common area of the supporting walls along the bend axis, and a square relief is added to the bend extremity. The Length 1 and Length 2 parameters can be modified if needed.
    Round reliefThe bend corresponds to the common area of the supporting walls along the bend axis, and a round relief is added to the bend extremity. The Length 1 and Length 2 parameters can be modified if required.
    LinearThe unfolded bend is split by two planes going through the corresponding limit points (obtained by projection of the bend axis onto the edges of the supporting walls).
    TangentThe edges of the bend are tangent to the edges of the supporting walls.
    MaximumThe bend is calculated between the furthest opposite edges of the supporting walls.
    ClosedThe bend corresponds to the intersection between the bends of the two supporting walls. The closed bend extremity lies on the surface of the encountered bend.
    Flat jointThe two bends are joined in flat view.

Manage the Unfold Method Parameter

You can specify the unfold parameter corresponding to the defined unfold method on a bend coming from the extrusion of a circle, or on a bend that is automatically computed.

  1. Select the sketch.
  2. From the Model section of the action bar, click Extrusion .
  3. To generate the bends's fillet, select the sharp vertex common to the two edges.
    All the vertices or edges that you choose for a specific unfold parameter value are added to the Bend geometry list in the Bend parameters frame.
    Notes:
    • If there are several elements, select the text corresponding to the unfold parameter in the work area to update the list with the appropriate geometry. For all the other bends, if no specification is given, the unfold parameter follows either the rule defined in the Sheet Metal parameters or the bend table, provided it is set in the Sheet Metal Thickness table.
    • If the extrusion contains non canonical edges, the K Factor applied to the resulting face will always be 0.5.

Manage the Extrusion Connections

You can control the connection of the extrusion with the shape using a face to tear.

  1. Create a sketch in the 3D area as shown below.

  2. From the Model section of the action bar, click Extrusion .
  3. In Merge Options, click the Contact faces box and select a lateral face in the work area.
  4. Click OK.


  5. From the standard area area of the action bar, click Fold/Unfold .


    Note: If an area of the extrusion overlaps the Sheet Metal shape, it cannot connect the shape.