so I have a customer part and I can not offset the surfaces at 0.00 so I can do my die design how do I work around this? some of the face I can not even pick I need to start this design now and I am not sure how cause I can not do anything, Please help.
Hi Travis,
Have you tried after importing to run import diagnostics?
Or if not, tools>evaluate>check?
There appears to be an open surface and a couple of general faults, I would first work on fixing these.
Thanks, Kyle
I did it twice and the bad faces I can not even delete.
Hi Travis,
Please see my attached model (2018).
I had to use delete and fill faces on the faulty faces found through the check tool, which are caused by the fillets.
Every surface can now be copied.
Thanks, Kyle
Is that something that they fixed in 2018 cause I have 2015 and I tired that it would not work. I had a Total of 6 faces I could not fix.
When doing the delete and fill, I had to select the face next to the faulty one, that creates that full portion of the fillet. Please see screenshot. I did this for every faulty face.
Thank you I will Try all of this.
There are corner filleted faces on your model that are causing the errors. Multi-Select both those faces, delete, then you the filled surface after. It should get you a good solid. I can post the model if you need. After working on your part a little longer, I would do this to every corner filleted face that is split in two. Even if import diagnosis doesn't catch it up front, it's going to cause you issues later.
Hi Travis,
Use import diagnostic and Evaluate and isolate the areas with issues. Then Split the overall body up in smaller bodies around the errors.
Export the faulty body out and work to fix the errors. Then import it back in. Much faster then keep messing in the original.
Check with evaluate to see if SW picks up issues.
Elmar
Sorry what do you mean split it up in smaller bodies this would be really useful information. Thank you
Hi,
Run import diagnostic. See where your model has errors. Now cut extrude the affected area out and save it as 1.x_t.
Then edit the cut extrude and select "flip side". That should give you the cut out body. Save it out as 2.x_t.
Import the file and run import diagnostics. Fix the errors. If it works then you should have on body without errors and another with.
Now you can fix the faulty section without having to work in a large component. Then save out the fixed body.
Finally import both bodies and merge. Now you should have a working model.
Use Import Diagnostic after import part is modified ... is also of interest if you happen to find errors after you have edited the dumb solid.
Elmar
Thank you!
I did fix it withSWX2016 and saved it as x_t. Give a try on this one
I think I understand how to fix this, But yours came out pretty good what did you do to make this work well?
I found the bad faces and delete them after that, I used boundary surface to fill them in.
Hi,
Run import diagnostic. See where your model has errors. Now cut extrude the affected area out and save it as 1.x_t.
Then edit the cut extrude and select "flip side". That should give you the cut out body. Save it out as 2.x_t.
Import the file and run import diagnostics. Fix the errors. If it works then you should have on body without errors and another with.
Now you can fix the faulty section without having to work in a large component. Then save out the fixed body.
Finally import both bodies and merge. Now you should have a working model.
Use Import Diagnostic after import part is modified ... is also of interest if you happen to find errors after you have edited the dumb solid.
Elmar