Bug - Sheet Metal Solid doesn't Follow Default Rule with Second Derive Part

[andrewdroth]

I'm using multi body sheet metal part to push solid bodies to parts in an assembly.

Due to the complexity of the original master part I opted to create a second master for defining the cut profiles needed.

My parts now pull from two derived parts, one pulls the solid body, the other pulls sketches for cut features.

Now I've run into a major bug. The solid in my part will not stay tied to the default sheet metal rule. Whenever I update either of the master parts, all of my derived parts uncheck the 'Follow Default' sheet metal settings, and therefore all of my flat parts are now broken.

I need to be able to lock that setting. How can I fix this?

 

[johnsonshiue]

Hi Andrew,

This is indeed a bug. I can reproduce it on my machine. The only workaround I can find is to edit each Derive node and uncheck "Link sheet metal styles" option. It seems that when there are two sheet metal source parts derived into one sheet metal part, "Follow default" will be unchecked on update for no apparent reason.

This is a very good catch. I will work with the project team to understand this behavior better.

Many thanks!

[tony]

Hi Johnson,

Has there been any progress on this, I'm having the same issue. Just installed 2019.1 this morning but no change in behaviour.

Thanks,

Tony

[johnsonshiue]

Hi Tony,

I will need to check with the project team. I thought this issue was resolved on 2019.1 but I could be wrong. I will get back to you with my findings.

Many thanks!

[dave_oliver]

Hi Johnson,

Any progress with this issue.

I'm working on a job that has nearly 100 sheet metal panels and I currently have to fix each one individually each time there is a small change.

Cheers

Dave.

[johnsonshiue]

Hi Dave,

I could be wrong but I don't think the issue you are having is the same as the original issue here. Andrew is using an unique workflow deriving two different sheet metal parts into one sheet metal part. There is a little bit styles collision here.

But, I assume your case should be straight forward meaning each derived sheet metal part contains a body linking to a master sheet metal part. Is it true? Have you install all relevant updates (2018.3 followed by 2018.3.4)?

Many thanks!

[dave_oliver]

Hi Johnson,

Thanks for your reply.

Yes, sorry you're right, my problem is as you describe, a part derived from
a master sheet metal part.

Yes, all updates for 2018 installed. I've now installed 2019 and migrated
the project to see if the problem still exists. I still have the same issue.

Cheers, Dave.

[johnsonshiue]

Hi Dave,

Did you install 2019.4? I recalled it was fixed in one of the updates but I don't remember the exact update. If it still not working on 2019.4, please share an example with me directly (johnson.shiue@autodesk.com).

Many thanks!

[dave_oliver]

Hi Johnson,

No, I hadn't installed any updates for 2019 as yet.

I'll do that and let you know how it goes.

Thanks for your quick response.

Cheers, Dave.

[andrewdroth]

@johnsonshiue 

This is still an issue in 2019.4

[johnsonshiue]

Hi Andrew,

The issue got addressed in 2019.2 was that we used to uncheck the option after the user did Make Components or other similar workflows. That was wrong.

For this particular behavior, you derive one sheet metal part and then another sheet metal part. Unless the two sheet metal parts share the same active style, "Follow default" will be wrong to the second derived body. This is why the option is unchecked on the second derived body.

Many thanks!

[klaashaesen]

This bug still seems to exist. I am working with Inventor 2019.4.1

I have a sheet metal part that is too long to make from one plate (14 m). So I derived it in a new sheet metal part and split the model to shorten it.

Then I derived a second ipt (not a sheet metal part, but a regular part) and use a sketch in it to make holes in my part.

I have one solid body and the sheet meal rule is set to "follow defaults". Everything works fine.

When there is an update to the original sheet metal part, Inventor decides to uncheck the option "follow defaults" and gives me an error.

I have used the same setup in my project 16 times. Which means I have to go into 16 parts and check the option again.

Is it possible to acces the "follow defaults" from ilogic or from VBA? Then I can try to find a fix while we wait for the bug to get sorted out.

[johnsonshiue]

Hi! Have you installed 2019.4? Did you create the part before 2019.4? Please share an example exhibiting the behavior.

Many thanks!

[MrCullen]

This is still an issue in 2021.2, the part was created in INV2020 and it was an issue in that release also. A sheetmetal part that is a derivative of a mirrored or derived part will uncheck the Follow sheet metal rule box when making an edit to the original.

Is there a fix to this? I find it hard to believe that Autodesk can not replicate this error and fix it within 3 years....

[A.Acheson]

I have seen this behaviour when changing back and forwards between standard and sheet metal part but not a derived part, haven't tried one of those. I think it  occurs at the selection of the first face prompt or just pressing ESC and not accepting any face. Which one is the cause, I will  need to check. Inv2020.4

[johnsonshiue]

Hi! There was indeed a fix to this workflow but it was not the exact same issue as discussed here. I believe there are multiple issues being discussed here. To avoid confusion, it is better to have an example that I can take a look. There should be a logical explanation. 

Merry Christmas and Happy New Year!

Many thanks!

[kimK7B54]

---

@johnsonshiue wrote:

Hi! There was indeed a fix to this workflow but it was not the exact same issue as discussed here. I believe there are multiple issues being discussed here. To avoid confusion, it is better to have an example that I can take a look. There should be a logical explanation. 

Merry Christmas and Happy New Year!

Many thanks!

---

Well, 4 years later and this issue still has not been fixed.  I/We have been using inventor 2021 for quite a while and we have been fighting this issue constantly; we are at the point we cannot use sheet metal functions that depend on having the correct thickness (i.e. "flange").  Personally, I think all the software people need to be replaced with competent people.  The never ending frustration with lack of support for buggy software has only getting worse. (perhaps a management change is in order)

[johnsonshiue]

Many thanks for sharing the files! I took a quick look and I think I know where the problem is. The Sheet Metal Rule management workflows in a multi-solid body sheet metal part can be confusing. This behavior has been discussed before. And, I was confused at a point also.

To certain extent, Sheet Metal Default is only relevant in a single-solid body part. It is a convenient way to change from one rule to another so that everything will update accordingly. Whenever there is more than one solid body, the default becomes meaningless. It will only work if all sheet metal bodies are in the same gauge. There are designs like that. But, more than likely in a sheet metal assembly, there can be multiple gauges.

The behavior you are seeing is actually a proactive way to avoid the default rule getting in the way. The original Sheet Metal Multi-Solid workflow assumes that you have multiple solid bodies and each is in the same or different gauges. Then you use Make Components command to push each solid body to a part. And, that is it.

However, in some cases the user may decide to derive another body (solid or surface) into the pushed body part. Essentially, the derived part itself may have multiple solid bodies also. This is where the confusion starts. As I mentioned earlier, when there are multiple solid bodies, the default is kind of irrelevant. The derived solid body has to be linked to the same rule as the source body. Otherwise, things will fail.

In your case, the failing sheet metal part does have two Derive features. As a result, Inventor clears out “Follow Defaults” option whenever there is a change coming from the source.

Thanks again!

[andrewdroth]

Hi @johnsonshiue,

Here's the issue as I see it. Please find the attached parts.

[NickdeNT2EU]

Inventor 2023 has the same issue. I have 98 sheet metal parts derived from a multi body master. Only one parts flat pattern breaks when updates occur and the other parts are fine. The follow defaults box has to be reselected in the select sheet metal rule to fix the problem but then breaks again the next time the multi body updates . First I suppressed the link to the multi body for the part which fixed the problem but is dangerous because you have to remember to unsuppress the link for the part to update. 

The fix for me was to edit derived part and go to options a deselect link sheet metal styles for the part I was having problems with.

Strange how only 1 of my parts is having issues and the rest are not