I created a new part via an extrude and then a number of cuts. After creating the part, I realized that I extruded in the wrong direction. In other words, I extruded "up" from the sketch plane rather than "down".
When I reverse the extrude, to extrude in the correct direction, almost all of my subsequent features fail.
How do I avoid this?
Thank you!
Jon
I'm not permitted to upload parts...
I assume that it may be possible to get permission to upload a parasolid file.
Jonathan Corsico - You need to edit the Sketch Planes of all the other Sketches and change the direction of Cut or Boss on the other features.. Then all will be well
John Stoltzfus wrote:
Jonathan Corsico - You need to edit the Sketch Planes of all the other Sketches and change the direction of Cut or Boss on the other features.. Then all will be well
No dice. Some of the features respond correctly to this, but many have sketch entities that just go crazy. For example, tangent relations will flip from one side of a spline to another. Other sketch entities will mysteriously end up way far away from the part!
1-8YRJL4N wrote:
How do I avoid this?
Going forward - use the BORN Technique as much as possible and practical.
Nearly all of my sketches are on the Origin planes.
It might be surprising what you can do - not using part faces as parents.
We're limited in how much help we can give without the file, other than using the origin and primary planes as much as possible, as J. Mather mentioned.
There's one other thing that may not help in your situation, but might help in the future. I often have construction lines in my sketches that I use to mirror and measure across. When I first started using SW I'd always fully restrain each end of these construction lines, and at least one end was usually coincident with a model edge. It wasn't uncommon for model edits further up the tree to cause that relation to fail, so I'd have to edit the sketch to fix it. I finally learned that as long as a construction line's position is fully defined the sketch will be fully defined, even if the end points aren't constrained. Since then I rarely fully define both end points, and that has saved me a lot of time.
Other than that, when modeling always keep the thought in the back of your mind that you may need to edit this model later, and plan accordingly. As with almost everything, that will get better with practice.
I am now able to post the file. Try to reverse the extrude direction of the first feature. Everything following it blows up!
Thank you!
Is this what you want?
Very clever! If I'm following correctly, you did a midplane extrude, and then cut off the half of the extrude that I didn't want. Right?
As another possible solution, I probably could have offset the extrude plane and then extruded in a single direction from that offset plane.
Thank you!
Jon
Yes that was the way I did. In your designing process you did not utilize origin planes.
With all that incontext stuff in there missing plane etc, It's just not worth fighting the software.
As Glenn Schroeder notes better to have a a construction sketch in there to reference plane etc from
At bottom of tree - Mirror bodies, then Delete original bodies.
1) All of the external references are locked. So I don't see why they should create an issue.
2) There are no missing planes. I'm not sure what happened in your part file, but everything is hunky dory on my end until I flip the direction of the extrude.
3) Good solution with the mirror & delete.
Thank you!
Jon
Hello,
Please upload your part so the replies can be more applicable.
How can I attach a file to a forum post?
Kevin