In Place Mate

[jwlynn64]

Has anyone ever heard of this?

I am working on an assembly created by someone else a couple of years ago.

I am getting an error when I try to change a dimension on one of the parts. When I look at the mates on the part, the only mate is an "IN PLACE" mate. I also get a dialog box telling me that this part is mated using "In Place Mates" and cannot be changed using the mates dialog box.

Any ideas?

John

 

[ctopher]

It is edited within the assembly.
Open assy, select part, edit part.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[Theophilus]

You can delete that mate (save a copy of your files first, just in case) and re-mate the part using standard mates. If you plan to move the part from its current position, understand that your sketch and other geometry that refers to other parts will get hosed. To avoid this, get rid of in-context stuff within sketches features first and then go back in and establish that stuff with real dimensions.

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[GTCadGuy]

John,
This part was created in the assembly on the fly, and was the first part in the assembly. The inplace mate is created between the front plane of the new part and the plane selected. You can look for this under help - in-context features, creating a part in an assembly.

See below from SW Help.

If the assembly is empty, select a plane from the FeatureManager design tree. Otherwise, select a plane or planar face on which to position the new part.

The name of the new part appears in the FeatureManager design tree, and a sketch is automatically opened in the new part. An Inplace (coincident) mate is added between the Front plane of the new part and the selected plane or face.

The new part is fully positioned by the Inplace mate. No additional mates are required to position it. If you wish to reposition the component, you need to delete the Inplace mate first.

Hope this helps.



SolidWorks 2006 - SP3.0
UG NX3
Pro/Engineer Wildfire 2.0

 

[jwlynn64]

Thanks to everyone for the info. I'll see about deleting it and adding other constraints.

John