Assy planes versus part planes

[gunnykiln]

OK, I have pulled all my hair out.

I created a master sketch in a new assembly file in the top plane. Then I used the sketch to create the individual parts from assembly. When I open the parts individually they are all screwed up. For instance I have a flat plate parallel with assembly top plane and the with the master sketch origin in the lower left corner. But when I open the part it is parallel with the front and the origin is in the upper right corner! What the hell? Do the assembly planes not match the part planes? If not how can I get them to match. I expected to see every part in the same orientation as I created them in the assembly file.

 

[CorBlimeyLimey]

Whichever face or plane you choose to create the new part on, will be the Front Plane of the new part. The Origin of the new part will be positioned at the perpendicular intersection of the assy origin & the parts creation face or plane.

To get around that problem, I usually create a blank part outside of the assy, insert it into the assy, & then create the in-context geometry. That way, the origin of the part is placed exactly where I want & the part is oriented correctly.
You could also use unconstrained geometry in the "blank" new part & then add in-context constraints after insertion into the assy.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[gunnykiln]

OK, is there any way to fix all the parts I have already created other than recreating them using your idea?

 

[CorBlimeyLimey]

Not if you want to maintain the in-context relationships ... that I know of anyway. Hopefully others here may have a workaround.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[StefanHamminga]

Try inserting your part on the assembly front plane, exit sketch, select the plane you want the actual geometry on and start a new sketch. That will make your parts appear exactly as in the assembly.

Existing parts: delete the in-context mate, mate the part the way you want and use the 'edit sketch plane' option


Stefan Hamminga
Mesken BV
2005 Certified SolidWorks Professional
Mechanical designer/AI student