Defective side after import diagnosis

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1

Hello

I have a part imported from UNIVER that has an error on one side.

No way to automatically fix the problem with "Try to fix everything" or by the advanced method.

I don't see what the problem is with this face (disjoint, hole, ?) and how to fix this error.

I attach the file:

 


chiusura_pneumatica_univer_ubp50ocu.sldprt
2

Hi Aliende,

Can you put us the swap file you downloaded?

3

Hi @ac.cobra,

I don't have the import file. It's an old project.
I have registered again on the UNIVER website but I have been waiting for their validation since yesterday.

Otherwise I would be curious to know how to repair this part myself because it happens from time to time to have files with this problem.

4

I think it must come from the hexagon because when I right-click on the error icon and I delete the face and I try to repair everything . Almost everything can be repaired except the hexagon...   see PJ


ac_cobra_427_chiusura_pneumatica_univer_ubp50ocu.sldprt
1 Like
5

Yes, that's interesting

I will take a closer look.

6

Otherwise by doing "Check entity", SW shows me:

7

Yes I've seen that too, I think he doesn't like the tangency of the edge of the plate and the screw.

2 Likes
8

Hello

It's the tangency between the flat face and the cylindrical face of the screw that he doesn't like, if you want to be able to repair this face you can add a little material on your part to extend your flat face then save in step, reload this step then redo the front repair and suddenly everything is repaired.

I'm attaching the step that I redid by extending the face by 0.1mm. I also redid the sldprt but I'm in 2017 and I saw that your piece was in 2016 so it won't be very useful to you.

Kind regards


chiusura_pneumatica_univer_ubp50ocu.step
2 Likes
9

Great @d.roger, the error has indeed disappeared!!

Did you extend the flat face into a surface? With what function?

Thank you!

10

Hello

No, I stayed on the basic, a sketch and then extrusion to the surface ...

I took this option but I could also have done a material removal on the diameter of the screw head. The goal is just to put a little material to avoid tangency between the edge of the face and the diameter of the screw head.

Then step recording, opening of this new step and repairing it...

Kind regards

1 Like
11

And to see the problem:

The result is that:

It's the same type of message as on sketches with intersecting profiles or tangent edges, to check you can make a sketch on the orange side, project all the edges of this face onto it, try to make an extrusion and there you find the tangency in question...

Kind regards

1 Like
12

OK
Thanks to you 2, I have a few files to retouch; This suits me because it's quite annoying these error messages that then end up in the sets and subsets.