How can I Edit Plane Definition but not move sketch.

[DigitalAssault]

Hi everyone.

I have several planes in my solidworks 2007 part file that were created by using definition points from surfaces that were initially brought in from an iges file. These planes were used to create my sketches on which I extruded my geometry. Unfortunetly a number of the surfaces that were used as definition points for these planes are now deleted so, although the planes are currently in the right place I have those bright red x's outlining the troubled planes. I can simply re-define the planes by editing the feature so they are defined from 'parallel planes from a point', however, when I do that the sketches and geometry I created on those planes often move way off the part and I have a hard time re-locating the sketches back into the correct place. Is there a way I can re-define the planes my sketches are on without my sketches moving away from there correct position in the part?

Thanks for any help you can provide!

David

 

[TheTick]

Add constraints and dimensions to your sketches to anchor them to something that is not moving, like principle planes and the origin.

 

[EEnd]

SolidWorks planes have a red side and a green side. What may be happening is that when you are redefining your planes, the red and green sides get flipped, throwing things off.

Eric

 

[dogarila]

Try to "fix" the geometry of the sketch before redefining the plane.

 

[DigitalAssault]

I fixed the sketch and that made no difference. The entire sketch stayed intact but was moved to another location once I re-defined the plane.

 

[fcsuper]

I think the issue may require someone asking, why do you need to move the plane but not the sketch? Are you trying to affect another feature, but two features refer to the same plane?

If so, you can change the plane your sketch refers to. I would create a new plane that is equal in location to the current plane. Then, change the plane that the sketch refers to from the current plane to the new plane. After that, the current plan can be moved without affecting the sketch.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[TheTick]

I believe fix works relative to the plane's origin for a 2D sketch, which may or may not coincide with part's origin.

One trick is to create a "backup" of your sketch. Create a 3D sketch, use "convert entities" to copy the 2D sketch entities, then delete all constraints in the 3D sketch before closing it. Now you have a copy that you can move up the feature tree and use as a template for comparing before and after.

 

[DigitalAssault]

Hey Matt,
I just tried what you suggested. Instead of re-defining the existing plane I created a new plane in the correct location with the correct definitions, then changed the sketch plane for the sketch that was on the broken plane. After that I erased the broken plane which I no longer required and it worked! My geometry is in the correct place and on a properly defined plane.

Thanks!
David

 

[dogarila]

So a star for Matt, I guess!!!