Delete hole from a surface body

[Anonymous]

Hi,

in Inventor 2018 is it possible to delete a hole from a surface body like this ?

It's a command that automatically patches a hole but creates a unique face.

It's like the surface "remembers" its shape before a hole was trimmed on it.

Thanks,

Alex

[kelly.young]

@Anonymous have you tried using the Surface > Repair Bodies?

About the Repair Environment

There might be combination of the surface commands that could produce meaningful results.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue]

Hi Alex,

For solid body, you can use Delete Face -> check Heal option -> select the faces to delete. For Surface body, you will need to use Repair Environment like Kelly mentions here. In RE, use Extract Loop command to restore the base surface.

Many thanks!

[Anonymous]

Hi,

thanks for your suggestion. I tried using closed loop command in construction environment, but I can't choose the hole loop I want. See here:

This generates surfaces that overlap.

Is there a way to select only hole loop ?

I'm attaching the file containing the surface.

Thanks,

[johnsonshiue]

Hi Alex,

This one can be a bit tricky to do. It is because the hole spans three different faces as opposed to just one. You can still use Extract Loop to do that. But, you will need to create new 3D sketch to reconstruct the loop. The process can be a bit tedious.

The quickest way seems to use Extend Surface command. The preview may look funny but the result will be correct.

Many thanks!

[WHolzwarth]

I tried in 2017 adding two arcs at the circular edges, and using Boundary patch with rails, but that failed. IMO it should have worked.

But have a look at another way of getting clean faces back.

2017 IPT attached.

[Anonymous]

Hi Johnson,

I tried extend surface. It almost closes the hole, but if you put a value that is larger than hole gap (e.g. 19,4 mm) it previews a strange surface but then doesn't close the hole:

The max I could get to was a very thin hole by using a 19,31 mm in the extend surface command:

I've created a 3D sketch copying the gap profile.

I was hoping extract closed loop would recognize it, but it doesn't because contruction environment comes before the 3D sketch:

[Anonymous]

Hi,

I've done a desperate attempt with the procedure shown in the video.

Basically I'm using the extract closed loops to untrim surfaces where I want to delete the hole.

Then I'm doing some trimming respect to existing geometry in order to restore original shape.

Finally I wanted to make some cleanup by deleting surface bodies that I used in modeling, leaving only the surface body with closed hole.

Iìm expoting the file to step and then importing it back again.

Unfortunately there are some errors, probably because of the small body that became a torus during untrimming operation and because of my modeling which wasn't exact.

Isn't there a faster procedure ?

I've checked also in Fusion 360 but you don't even get an untrim command there.

[catot]

If I understand correctly, the Patch-command should work for this? (on surface panel).

[torbjorn · Accepted solution]

Not very intuitive, but the surface can be generated via a solid:

- Thicken the complete surface to a few mm solid

- Delete faces in the hole, check heal

- Thicken a new surface, 0 mm offset from the original face

Torbjørn

[Anonymous · Accepted solution]

Torbjørn,
I like it, it's a very creative approach !
It seems that with solid modeling you can overcome limitations in surface modeling with Inventor.
Below you can see the video of the procedure described by Torbjørn.

All credit goes to Torbjørn, thank you again!

[WHolzwarth · Accepted solution]

[Anonymous]

Sorry torbjorn,

but credit to the solution goes to Walter because actually he was the first one to propose a solution like yours.

Sorry Walter, I didn't see the attachment.

Now I realize you're the first one who gave the solution.

[WHolzwarth]

Only a minor problem, Alessandro. You're welcome.