Create and modify 3D models > Make a 3D model > Pull a part (Pull Linear)
  
Pull a part (Pull Linear)
Pull () allows you to:
• Create a solid part by lifting a 2D profile into a solid object. This operation adds material to a part.
• Remove material from a part or a face.
The Pull operation supports Profile handling.
Add Material
Remove Material
To pull a part (from a profile),
1. Click Modeling and then, in the Model group, click the arrow next to Pull.
2. Click Pull Linear. The Pull dialog box opens.
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By default, Profiles is selected in the Pull dialog box.
3. Select or type a Part name.
4. Select the workplane either in the viewport or the Structure Browser. All profiles on the workplane are machined.
5. Click Selected to choose specific areas of the profile on the workplane.
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The default option in the Operation box is Automatic. Creo Elements/Direct Modeling automatically selects the most likely operation based on the other options in the Pull dialog box. You can also choose Add Material or Remove Material in the Operation box if the system suggested operation is not the wanted operation.
6. In the Type box, select a pull mode:
◦ Distance: a distance through which to pull the part.
◦ To Part: an existing part to which the new part is pulled. The profile must not extend beyond the boundary of the part.
◦ To Faces: a face, set of faces, or face part to which the new part is pulled. The profile must not extend beyond the boundary of the face(s).
◦ To Point: a point on a part or in a workplane. The profile is pulled until the pull direction is perpendicular to a line projected through the point.
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The To Point option is available only when you pull a profile.
◦ To Plane: a plane defined using the Axis 3D tool. The profile is pulled until it intersects the plane. This extrusion mode can, therefore, generate a part with an angled surface.
7. Set the Draft Angle. The lateral faces are tapered along the pull direction by this angle.
8. Set the Direction:
◦ +w: Positive normal direction of the workplane containing the profile.
◦ -w: Negative normal direction of the workplane containing the profile.
◦ Both Sides: Both sides of the workplane containing the profile.
◦ User Def: Direction defined using the Direction 3D tool.
9. Select Keep WP to keep the workplane and/or Keep Prof to keep the profiles used. Deselect either of these options to discard the workplane or profile after you pull.
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To toggle between Realistic Feedback and quick feedback, see Change Modeling settings.
10. Click to complete the operation.
To pull a part (from a face),
1. Click Modeling and then, in the Modify 3D group, click the arrow next to Modify.
2. Click Pull. The Pull dialog box opens.
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By default, Faces is selected in the Pull dialog box.
3. Select a face of a part in Viewport.
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The default option in the Operation box is Automatic. Creo Elements/Direct Modeling automatically selects the most likely operation based on the other options in the Pull dialog box. You can also choose Add Material or Remove Material in the Operation box if the system suggested operation is not the wanted operation.
4. In the Type box, select a pull mode:
◦ Distance: a distance through which to pull the part.
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If you choose Distance, you can use Next to pull a face in multiple stages. The most recently pulled faces remain selected and you do not need to restart the selection. You can also use Back to go back one level.
◦ Dimension: 3D Annotation (dimension) connecting the faces that can be pulled.
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• The Dimension option is available only when you pull a face.
• If you choose Dimension in the Type box, you can type the distance for pull in the Distance box. The dimension automatically defines the pull direction and sets the initial distance value from the dimension value.
◦ To Part: an existing part to which the new part is pulled. The profile must not extend beyond the boundary of the part.
◦ To Faces: a face, set of faces, or face part to which the new part is pulled. The profile must not extend beyond the boundary of the face(s).
◦ To Plane: a plane defined using the Axis 3D tool. The profile is pulled until it intersects the plane. This extrusion mode can, therefore, generate a part with an angled surface.
5. Set the Draft Angle. The lateral faces are tapered along the pull direction by this angle.
6. Set the Direction:
◦ +Face Normal: Positive normal direction of the face.
◦ -Face Normal: Negative normal direction of the face.
◦ User Def: Direction defined using the Direction 3D tool.
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• To toggle between Realistic Feedback and quick feedback, see Change Modeling settings.
• You can click Chk & Fix if you suspect a part is corrupt. Chk & Fix checks for self-intersections, knife edges, and void shells and attempts to fix them. If a part fails the check and fix, it is not modified and remains in its original state.
7. Click to complete the operation.