Offset Expand Difficulties

[CarbonCAD]

I have a part that was sent in .stp format and it needs .003 removed from the outside of all surfaces. I have found that offset expand works well for me to do this. I now have a part that will not work with offset expand, because of where some radii meet. I have cut out the area of the part in question and attached the picture. Any suggestions on how to do this?

 

[solidworm]

i guess the problematic area has a degenerate point which causes the offset not to work.
(see if view->model setup->mesh surface results to a mesh converged to a point on that surface)
you have to replace that face with a trimmed four sided surface.(created using boundary blend or VSS). i tried but couldn't come to an acceptable result. if nobody posted a solution , upload the file and i might be able to fix it using other tools.

Edited by: solidworm

 

[magneplanar]

CarbonCad,

test your offsets to find the specific surfaces that fail. (analysis-->geometry-->offset(select "quilt instead of the "smart" selection filter option)

You can then select and offset all the rest (seed and boundary...). After that you can rebuild that missing surface/s to complete the quilt as mentioned above.

Depending on your version, can you suppress the rounds? Are their flaws in the import that you can repair with pro-e IDD?

cheers,

M

 

[jeff4136]

Another thing to look at if you're using Relative Accuracy is the
current effective accuracy. Change to Absolute, use the From Model
option and select the current model from In Session to determine.


You really should post the geometry set. There's probably half a
dozen reasons for failure, each with multple fix options that could
be pursued. Bottom line, though, is likely to be getting rid of the
offending surf(s) and recreating them. Looks like you should be able
to create new surfaces to sharp intersection and add new fillets.

 

[vitadj]

Try to use Remove feature to remove rounds in problematic area, then use offset expand 0.003 and, finally, recreate rounds with lower values for radius.
Remove feature resides in Edit menu, but first you must select some surfaces.
It is feature with awesome results.


Edited by: vitadj

 

[design-engine]

If you are able to cut out the problem area then you now how to localize the problem.

You might also rethink your rounds so they do not go to a point like that. That's often a big problem with shelling products. I suggest using one radius for one direction rounds and another slightly different radius for the other direction rounds.Of course if your a typical tooling guy no one will listen to you.... then your stuck with what they give you so changing the rounds is not an option.

Edited by: design-engine