Creating Cutouts

You can create cutouts defined either by a sketch or an open geometry.

Creating cutouts consists in extruding a profile and removing the material resulting from the extrusion.

This task shows you how to:

Before you begin: Create a web containing a closed sketch.
See Also
About the Creation of Cutouts
Creating Holes

Create Cutouts Using a Sketch or a Wireframe Element

You can create cutouts using a sketch or a wireframe element.

  1. From the Refine section of the action bar, click Cutout .
  2. Click Standard .


  3. In the Profile box, select the sketch.
    The vectors show the side and the direction of the cutout.

    Notes: The following options are available:
    • Open catalog : Inserts a profile from a catalog.
    • Normal to profile direction : Positions the cutout direction perpendicular to the selected sketch.
    • Reverse direction : Inverts the direction of the extrusion.
    • Reverse material : Chooses between removing the material defined inside the profile, which is the default behavior, and removing the material surrounding the profile.
  4. To define the limits, select the type and its associated parameters:
    OptionDescription
    Dimension Creates the cutout using a depth value.
    Up to next Creates the cutout up to the next surface.
    Up to last Creates the cutout up to the last surface.
  5. Enter a length for each limit.
  6. Optional: To manage the impact of the cutout results, select your options:
    OptionDescription
    Optimize Geometry Improves the result of the cutout by taking into consideration impacts on both the top and bottom faces.
    Note: You cannot use this feature when the cutout result impacts complex geometry (such as propagated flanges, or stamps).
    Faces Specifies the faces for which you want to manage the impact of the cutout result.
    Gap Specifies the gap between the input surface and the cutout result, when Optimize Geometry is selected.

Create Pocket Cutouts

You can create pocket cutouts on a planar and single support surface.

Before you begin: Create a sketch.
  1. From the Refine section of the action bar, click Cutout .
  2. Click Pocket .
  3. Select the sketch as the profile.
  4. Specify the limit values.
  5. Optional: To manage the impact of the cutout results, select your options.



Warning: You cannot create a standard cutout on a pocket cutout or on a feature impacting a pocket cutout.

Create Cutouts from an Open Profile

You can create an open cutout by thickening the profile.

  1. From the Refine section of the action bar, click Cutout .
  2. Click Standard .
  3. In the Profile box, select the open sketch.
  4. Click Thick profile.
  5. Define the thickness values:
    OptionDescription
    Thickness1 Impacts the outside thickness of the profile.
    Thickness2 Impacts the inside thickness of the profile.

    You can click Equal thickness to create a cutout whose thickness is the same on both sides of the sketch.

Create Cutouts for a Cylinder

To get a cylinder through a Sheet Metal part, you can create a cutout on both the bottom and the top skin.

  1. From the Refine section of the action bar, click Cutout .
  2. Click Standard .
  3. From the 3D area, select the cylinder to pass through the Sheet Metal part.

    Warning: The Limits and Direction boxes are unavailable.

  4. To take into account only the part of the sketch that lies on the top or bottom face, click Lying on skin.
    Created Cutouts

    Drawing View of 3D Shape

  5. Optional: To manage the impact of the cutout results, select your options:
    OptionDescription
    Optimize Geometry Improves the result of the cutout by taking into consideration impacts on both the top and bottom faces.
    Cutout with an impact on the top face, without Optimize Geometry selected

    Cutout with Optimize Geometry selected

    Note: You cannot use this feature when the cutout result impacts complex geometry (such as propagated flanges, or stamps).
    Faces Specifies the faces for which you want to manage the impact of the cutout result.
    Gap Specifies the gap between the input surface and the cutout result, when Optimize Geometry is selected.

    Cutout with Optimize Geometry selected, and Gap specified