Creating an Extrusion

You can add a material to an open and planar sketch profile.

For learning module and videos of extrusion, refer > Explore the 3D SheetMetal Creator Role > Using Extrusion and Wall on Edge .

This task shows you how to:

 

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Create an Extrusion

  1. From the Sheet Metal section of the action bar, click Extrusion .
  2. In the dialog box, click Profile, and from the work area, select an open sketch as a profile.

    Select an open sketch for extrusion.

  3. Click Fixed geometry, and from the work area, select an edge or point as a reference.
  4. From the Sketch Orientation list, select one of the following:
    OptionDescription
    Inside Orients the sketch at the inside position of the wall thickness.
    Middle Orients the sketch at the middle position of the wall thickness.
    Outside Orients the sketch at the outside position of the wall thickness.
  5. For Direction 1 and Direction 2, specify the direction of an extrusion by selecting one of the following:
    OptionDescription
    Dimension Extrudes a selected profile on one direction.

    If Dimension is selected for Direction 1, select Symmetric for Direction 2.
    Midplane Extrudes a selected profile on mid plane.

    If Midplane is selected for Direction 1, Length is equal to total length of extrusion.
    Symmetric Extrudes a selected profile on two opposite directions.

    This option appears only if Dimension is selected for Direction 1. If the Symmetric option is selected for Distance 2, Length equals half of total length.
    Up to plane Extrudes a selected profile up to the plane.
    Up to surface Extrudes a selected profile up to an existing surface.
  6. Specify a Distance from the selected profile to create the extrusion.
  7. Optional: Under Bends, select Automatic Bend to specify the bend extremities for Relief 1 and Relief 2 using one of the following options:

    By default, Automatic Bend is selected.

    OptionDescription
    Minimum with no relief The bend corresponds to the common area of the supporting walls along the bend axis, and shows no relief.
    Square relief The bend corresponds to the common area of the supporting walls along the bend axis, and a square relief is added to the bend extremity. Length 1 and Length 2 parameters can be modified.
    Round relief The bend corresponds to the common area of the supporting walls along the bend axis, and a round relief is added to the bend extremity. Length 1 and Length 2 parameters can be modified.
    Linear The 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).
    Tangent The edges of the bend are tangent to the edges of the supporting walls.
    Maximum The bend is calculated between the furthest opposite edges of the supporting walls.
    Closed The bend corresponds to the intersection between the bends of the two supporting walls. The closed bend extremity lies on the surface of the bend.
    Flat joint The two bends are joined in a flat view.

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

    Linked to SheetMetal parameters shows that the given parameter is driven from global sheet metal parameters. You can click to unlink it. shows that the given parameter is a local or custom value.

  8. Under Custom bend calculation , click Bend geometry and from thework area, select a vertex.
  9. For Bend calculation, specify a value for K-factor.

    You can create multiple K-factors for multiple bends.

    Click Linked to SheetMetal parameters next to K factor to get the options, Bend Allowance and Bend Deduction for bend calculation. Specify the value for bend allowance or bend deduction.

  10. Click to save and exit.
    Note: You can use equations for all numeric parameters in this feature. Click the dimension text. The dimension text becomes editable. Type = in the input field, to open the Equation dialog box and enter a formula or number. From the list, select a parameter. You can perform the basic operations such as addition, subtraction, multiplication, and division on the parameter value.

Create an Extrusion by Dragging

You can drag the arrow handle in the sketch to extrude. This works only for the open sketches and not for the closed sketches.

  1. From the Sketch section of the action bar, sketch an entity.
  2. Click the entity and drag the handle that appears.
    A mini panel appears.

    Specify the extrude distance by dragging the arrow, then slide the indicator on the ruler to snap to rounded-off values, or enter a value by double-clicking the number.

  3. From the Sketch orientation list in the context toolbar, select one of the following:
    OptionDescription
    Inside Orients the sketch at the inside position of the wall thickness.
    Middle Orients the sketch at the middle position of the wall thickness.
    Outside Orients the sketch at the outside position of the wall thickness.
  4. From the mini panel, select Midplane to create extrusion equally to both directions from the midplane.
  5. To expand the Extrusion dialog box, select Expand.
  6. Click OK .
    The extrusion is created.

Manage Extrusion Connections

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

  1. Create a sketch in the work area.
  2. From the Sheet Metal section of the action bar, click Extrusion.
  3. In the Extrusion dialog box, click Select profile.
  4. From the work area, select a profile that connects two faces.
  5. Click the Fixed Geometry.
  6. From the work area, select a point or edge of a profile.
  7. Under Merge Options, click Contact faces.
  8. From thework area, select faces that the profile connects.
  9. Click to save and exit.