idw visualization error of a imported step

[Christian_1976]

Good morning,

I imported a downloaded stp part (motor) and i made an ipt from the iam import result.
(i did not flag "surfaces" in import settings.)
I also "save as" the ipt, breaking the bindings from the iam to make it standalone.
Then I placed the motor in an assembly of my pump.
Also here, i made a derived part of the pump and i used it in another assembly.
When i make an idw I got a strange behavior, maybe due to an import error or source model error;

it shows me a semicircle around the motor and it hiddens the lines behind, like it were solid.
I can hide the semicircle line but it still hides behind.
If i choose to see the view as "rendered/colored" it didn't hides behind (only the black objects edge is missing).
I checked the imported file more times but i can't see this hidden line or surface in any place.
It seems clean to me.

Any idea about how to fix it?

Or maybe the best thing is to don't waste more time on this and use a dummy ugly motor?

Thank you

kelly.young has embedded your images for clarity.

[johnsonshiue]

Hi! This is geometry specific issue. Basically, Inventor drawing has trouble showing the silhouette edge of the model. Try this. Edit the view and go to Display option -> check Tangent edges. If it does not help, please share the file here or send it to me ([email protected]). I can try and see if Repair geometry workflow will help.

Many thanks!

[Christian_1976]

Hi,

thank you for the reply,

"tangent edges" was already selected.

I tried to play with options but nothing changes.

I can send the motor file, do you want it in source step or iam/ipt converted from?

Thank you

[Christian_1976]

Hi, i found a workaround.

I re-imported the step file keeping separate solids.

Then i searched for the subpart that was causing the issue.

Found that subpart, but after checking that all was normal (at least it seems) i saved as stl and reimported and then converted with mesh enabler.

Made a substitution in motor assembly and the problem was solved.

I attach here the step. The faulty sub part is named "B3100" after import. (Making an idw with this part shows you the issue)

Thanks!

[johnsonshiue · Accepted solution]

Hi Christian,

Yes, you are right. The issue is indeed with "B3100." The geometry checks fine but the edges shown in the attached image do have a gap about 0.00005mm exceeding Inventor modeling tolerance (10E-5mm).

There are two ways to fix the issue. 1) You can simply right-click on the big arc edge in the drawing -> uncheck Vibility. Or, 2) Open the part and find the edges shown in the attached image. Use Delete Face command -> select either side of the torus faces (just select one but not both) -> check Heal -> Ok. After that, you will see the big arc edge will go away.

[Christian_1976]

Hi Johnson,
I'm replying to thank you in the first,
then i only want to say that hiding the arc uncheking the visibility doesn't solve the issue. (was my first try)
I'm more interested in the second "magic" solution. I'm totally unprepared to work with surfaces and this side of Inventor, so it makes me curios and i eager to learn, so i will try to fix it (*oculus reparo* :D) also if I already solved with a workaround.

Thanks again