topic Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid) in Inventor Forum

Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Wed, 03 Jul 2024 21:04:50 GMT

Dear @johnsonshiue
I'd like to know why Inventor fails to create flat pattern for the flat models like attached* (pops "The input body is invalid" message)

It does contain Flat pattern but this was achieved with playing around with parameters.

If removed can't be re-created.

PS:
The issue is reproducible in all releases I've checked till now, which are:

2023.4.2

2024.3

2025.0.1

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

SBix26 — Thu, 04 Jul 2024 17:45:05 GMT

Very strange! Using Inventor 2023.4.2, if I pick the entire profile for the Face instead of just the ring shape, making it a disk, Inventor has no problem creating a flat pattern. If I then remove the center profile, the flat pattern remains valid. This is true whether using Face & Cut or two Extrusions. I have no idea why that would be.

Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Thu, 04 Jul 2024 17:49:35 GMT

There is one more layer in this puzzle:
Inner dia is 30mm
Outer dia is 46mm
Half of the difference equals to the Thickness (both are 8mm)
If make them different (let say change outer dia value to 45mm) then Flat Pattern create is OK.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Frederick_Law — Thu, 04 Jul 2024 18:03:52 GMT

It pick wrong surface for "A Side". It try to pick "smallest" thickness.

Define "A Side" and it won't fail.

You'll see what IV try to do if you cut the ring in half.

See attached.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Thu, 04 Jul 2024 18:11:52 GMT

Here is a misunderstanding. I don't meen to produce this part with bending.
It is supposed to be lazer-cut from the 8mm sheet thus need to have Flat Pattern.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Frederick_Law — Thu, 04 Jul 2024 18:16:15 GMT

No misunderstanding.

That's how IV flat pattern work.

It failed because it cannot flatten a circle. It picked wrong A-Side.

No A Side defined:

A Side defined:

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Thu, 04 Jul 2024 18:22:26 GMT

Why it don't allow to pick (use) the red face as A-side? (like it does when dia difference differs from the Thickness) ... that is the question.
For me this limitation sounds like software defect.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Frederick_Law — Thu, 04 Jul 2024 18:33:57 GMT

I can pick red face as A Side. 2023.4.1

Need to delete Flat Pattern first.

Yes, IV "should" be able to pick correct face.

Only if programmers can find all the cases that cause it to fail and don't cause other problems.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Thu, 04 Jul 2024 19:25:11 GMT

Pure 2024 (as well as 2024.3) allows to pick for A-side only either of the two cylindrical faces ...

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

SBix26 — Thu, 04 Jul 2024 22:02:13 GMT

In 2023, if I select the Define A-Side tool, I cannot select either of the two flat faces (because they have no bends, I guess). However, if I select one of the flat faces and then invoke the Define A-Side tool, it applies the A-side definition as I asked and produces the proper flat pattern.

I think you have happened upon a really unique "fault" in the sheet metal logic. There are several methods to work around this, so it's not a showstopper. It's rare to produce a flat pattern of a part that has no bends, and it's rare for a sheet metal part to have a uniformly "bent" feature that matches the part thickness. Very entertaining!

Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

johnsonshiue — Mon, 08 Jul 2024 23:09:56 GMT

Hi! I believe the only way to create the Flat Pattern on this particular part is to create a full circular plate and create the flat pattern. Then edit the Face feature and remove the inner circular profile.

The reason the Flat Pattern fails is because the body has equal thickness in each way Inventor measures. Inventor cannot distinguish which face to start the Flat Pattern.

When the inner circular profile is removed, the circular plate has a logical thickness. As a result, the Flat Pattern works. Since it works, the starting face has been identified and it does not matter how the Face is changed (with or without the inner loop).

The behavior has been consistent. I am also able to reproduce the behavior on 2020.

Many thanks!

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Maxim-CADman77 — Tue, 09 Jul 2024 06:59:28 GMT

Dear @johnsonshiue
There is no need to change geometry.
There have been already found the easier way - select flat face then press "Define A-side" button. Then flat pattern is OK to be created
The bad thing about this - Inv don't allow to do it in normal way (first activate A-side command and than pick a flat face) which is very confusing.
With this in mind I still believe this is the defect and should be fixed.

Re: Inventor fails to create flat pattern for part with flat topology (The input body is invalid)

Bearded_Engineer — Tue, 08 Oct 2024 13:58:48 GMT

Just had the same issue, if you create a ring with inner size X and offset of X is equal to the sheetmetal thickness it will fail to create a flat pattern. Even when the part is much large in surface area then the thickness. Very strange behaviour, almost as if Inventor is trying to unfold the closed ring through it's sidewall. (Would understand the behaviour if the ring would have a split somewhere.)