Profile Center Mate
Profile Center Mate automatically center-aligns geometric profiles to each other and fully defines the components.
To create a profile center mate:
-
In an assembly document with two rectangular or cylindrical
profiles, click Mate
.
-
In the PropertyManager,
on
the
Advanced
tab, click Profile
Center
.
- For Entities to Mate, select the edges or faces that you want to center-align.
-
In the PropertyManager, you can optionally:
- Change the mate alignment by clicking Aligned
or Anti-aligned
.
- Change the orientation to Clockwise
or Counterclockwise
.
- Offset the two mated entities.
- For cylindrical profiles, click Lock Rotation to prevent the components from rotating.
- Change the mate alignment by clicking Aligned
-
Click
twice to close the PropertyManager.
Profile Center Mate - Supported Profiles
You can use profile center mate for these types of entities:
- Full circular edge or face
- Linear edge
- Regular n-sided polygon edge or face
Rectangular profiles can have fillets, chamfers, internal cuts, or cut-off corners. You cannot use rectangles with cuts or additions to the perimeter for profile center mates.
| Supported profiles |
| Unsupported profiles |
For unsupported profiles, you can create a supported profile sketch to use in the profile center mate.
| Part with unsupported profile | Rectangular profile sketch mated to rectangular base using profile center mate |