Move part to origin

[difficultone]

I have a part that I received from a customer. The part has it's origin out in space. How do I move the portion of the part I want to use for an origin to the SolidWorks Origin? I created a Reference Geometry Coordinate System at the point on the part I wish to move to the SolidWorks Origin.

 

[Eltron]

You can insert the part into a new part and position it where you want it.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[difficultone]

Dan, How do I position the part once I insert it into the new part?

 

[Eltron]

When the insert part dialog comes up be sure the "Launch Move Dialog" in the Locate Part is checked.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[difficultone]

I used Move/Copy Bodies and the Measure tool and got the job done but what a PITA. Is there a tutorial available on using Move/Copy Bodies tool or some other tool that can be used to perform this function?

 

[CorBlimeyLimey]

difficultone,

If you have created a new coordinate system in the part, all you need do is Save as to a parasolid using the Option to use the newly created CS as the default. When re-imported into SW, the origin and CS will match. You will however end up with a dumb solid, but if you have the Feature Recognition module, features can be rebuilt.

A (usually) more involved alternative would be to re-assign sketches to the main reference planes. If you are very lucky, just re-assigning the base feature sketch will carry all subsequent features with it.