Push, pull, or revolve a face, sketch, line, or 2D edge to extrude it into a solid or surface, create or resize a hole, eliminate rounds, or modify wall thickness.

Push or Pull a Face, Line, or 2D Edge

Push or pull a face, sketch, line or 2D edge to extrude it into a solid or surface.

  1. Open the Push/Pull tool in one of the following ways:
    • Press P.
    • Double-click a part.
    • On the Geometry ribbon, select the Push/Pull Faces tool.

  2. Select a face, line, or 2D edge in the modeling window.
  3. Push or pull it in one of the following ways:
    • Drag the selected object. To make it a new part, select the icon on the microdialog or hold the Shift key while dragging.
    • Enter a precise distance in the microdialog. A positive value extends, whereas a negative value contracts.
    • Drag the gray pyramid on the ruler to position the start point for the measurement, then drag the white arrow or enter a value in the microdialog to position the end point.
  • Use snap points to align faces or subfaces so they are at the same level, or make one face flush with another. When pushing and pulling faces and subfaces, objects automatically snap to snap points such as end points, center points, quad points, and midpoints on other parts.
  • 2D edges can only be pulled, not pushed.
  • To place multiple solid bodies into separate parts, right-click on a part to open the context menu, then select Convert Bodies to Parts.

Push or Pull a Sketch on a Face

Push or pull a sketch on an existing face and create, modify, or replace the existing part.

  1. Open the Push/Pull Faces tool.
  2. Select a sketch on face in the modeling window.
  3. Drag the selected sketch. To make it a new part, select the + icon on the microdialog, then choose one of the following options in the pull-down menu:

    • New Part: Create a new part based on the pushed/pulled geometry.
    • Add to Part: Add the pushed/pulled geometry to the existing part.
    • Remove From Part: Remove the pushed/pulled geometry from the existing part.
    • Replace Part: Replace the existing part with the push/pulled geometry.

Revolve a Face, Sketch, Line, or 2D Edge

Revolve a face, sketch, line, or 2D edge about an axis.

  1. On the Geometry ribbon, select the Revolve Faces tool.

  2. Select a face, line, or 2D edge.
  3. To designate the rotation axis, select an edge, line, or cylindrical hole.
    Selecting an edge on another part projects the axis of revolution to the planar face that will be rotated.
  4. Choose from the following options:
    • Drag the face, line, or 2D edge.
    • Drag the white arrow on the compass.
    • Enter an angle in the microdialog.

    Figure 1. Revolving a Part
  • To create a new part, hold down Shift while dragging.
  • To reposition the axis of revolution using the Move tool, click in the microdialog.
  • Drag the rotation arrow by its midpoint to snap to snap points. Clicking elsewhere on the rotation arrow will temporarily disable snapping.
  • Selecting a face from a 2D sheet automatically revolves the face a full 360 degrees. Once you drag the face, the only way to get back to a full 360 degrees is to enter 360 in the microdialog.

Apply a Variable to a Parameter

Apply a variable to a parameter, or create a new variable on the fly from a tool microdialog.

You can apply existing variables and add new ones via the microdialog in various sketch and geometry tools.

  1. In the tool’s microdialog, click the f(x) icon.

    Figure 2. Example of a microdialog with a variable field
  2. In the dropdown menu, select Add Variable to create a new variable based on the dimension in the text field, or select the name of an existing variable.
  3. Click Apply to apply the variable to the construction feature.
  4. Right-click and mouse through the check mark to exit, or double-right-click.
  • You can also create a variable by entering a new name and expression in the microdialog’s text field, for example: Variable1=50
  • In addition, you can also create a new variable based on an existing variable, for example, Variable2=Variable1*0.5.

Maintain Snap Reference

Create and maintain a snap reference to another part.

You can link a pushed, pulled, or revolved construction feature to a snap reference point. As you make changes in the History Browser, the part will be automatically updated based on the position of the snap reference.

  1. Open the Push/Pull Faces or Revolve Faces tool.
  2. Click-and-drag the sketch or face you want to push, pull, or revolve. As you drag, move the mouse cursor over a snap point on a different part to snap to that point.
  3. Select the Maintain Snap Reference icon on the microdialog. The snap reference will be maintained as long as this option is enabled.
Tip: You need to drag the cursor toward a particular snap point on the other part, or the face will not snap. If the right snap is not becoming active as you drag, try rotating the view slightly.

Resize a Hole

Pull a cylindrical face to resize a hole.

  1. Open the Push/Pull Faces tool.
  2. Push the subface of a closed sketch inward until the hole penetrates the opposite side of the part. Change the diameter of a hole by dragging the interior face of the hole.

Eliminate Rounds

Remove rounds by pulling them into a sharp corner.

When you extend a face that has rounds adjacent to it, the rounds are moved with the face. Sometimes, complex rounds and blends will prevent a face from moving because they cannot be reconstructed at the desired position if the face is moved. If you do not care about retaining the rounds, you can often free up a stuck face by extending the round to eliminate it.

  1. Open the Push/Pull Faces tool.
  2. Select a round.
  3. Pull outward until the round is converted into a sharp corner.
Tip: If the face is a simple cylindrical round, the radius should change as you pull. If the round does not change, the geometry is too complex for the Push/Pull tool to modify.

Keyboard Shortcuts & Mouse Controls

To Do this
Activate the Push/Pull tool P or double-click
Temporarily disable snapping Alt
Make the object a new part Shift
Exit tool Right-click and mouse through the check mark to exit, or double-right-click.