topic Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked in Inventor Forum

Sheet metal style still linked after "Link sheet metal styles" is unchecked

jef.clissen — Tue, 31 Aug 2021 12:16:01 GMT

Hi All,

We've noticed when working with sheetmetal multi-body parts where a sheet Metal Default is selected. When making a derived part of a certain body were the thickness or material is not the same as the parent part we uncheck "Link sheet metal styles". This should, in our understanding, completely break the link of the sheet metal styles and just 'copy' over the geometry. Then we select the correct default in the derived part itself.

We're experiencing a bug were the 'Sheet metal default' of the derived part is being overridden by the default of the parent part. resulting in all sorts of problems (thickness, bending parameters and material are changed)

This bug happens when a geometry change is made to the exported body in the parent part. (dimension change or adding a hole...).

Has anyone else noticed this bug? If yes, is there a fix ?

Thanks in advance

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

johnsonshiue — Tue, 31 Aug 2021 19:29:01 GMT

Hi! I vaguely remember this is a known issue. The problem here is that the option pushes the sheet metal style to the derived sheet metal part. To avoid collision, it might be better renaming the style in the derived part. So that they are not the same named style. Otherwise, it can be confusing.

Many thanks!

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

jef.clissen — Wed, 01 Sep 2021 06:19:16 GMT

Renaming the style doesn't work. I don't understand how this is possible? I uncheck the 'Link sheet metal styles' checkbox but it still pushes the settings towards my derived part? It's not like they're the same styles in both parts (I understand that this might cause them to sync). They're different styles in both parent and derived part.(Can even be different materials). It still overrides the style i've selected in the derived part.

This is a major bug that can cause a lot of problems.

video:

https://autode.sk/3kL4IkO

thanks

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

johnsonshiue — Wed, 01 Sep 2021 18:11:59 GMT

Hi Jef,

Then the behavior sounds like a bug to me. If possible, please share the files with me johnson.shiue@autodesk.com. I would like to take a closer look.

Many thanks!

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

jef.clissen — Mon, 06 Sep 2021 07:28:28 GMT

I can't send the files i'm working on at the moment but i'll try to recreate the bug with some other files which aren't confidential.

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

P.DijkstraQLVKB — Fri, 06 May 2022 07:33:12 GMT

Has the above problem already been solved? I have the same problem with major consequences. All material thicknesses are adapted to that of the mother part. Only this should not have been the case and the checkmark at link sheet metal styles is unchecked. But still he changes all material thicknesses to that of the mother part.

Kind regards

Pieter jan Dijkstra

@johnsonshiue

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

jef.clissen — Fri, 06 May 2022 08:34:38 GMT

Not that I know.

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

johnsonshiue — Fri, 06 May 2022 20:40:23 GMT

Hi! The issue here is that when the sheet metal solid body is pushed to a derive part, the body thickness does not change because you assign a different sheet metal rule to the body. The thickness is the same as the source body.

You may think about this workflow similar to iPart paradigm. The source part is like the iPart factory holding the definitions of all the sheet metal solid bodies. The derive parts are driven by the source part.

Could either of you send me an example that exhibits the behavior? I don't recall I saw an example. I would like to confirm my suspicion.

Many thanks!

Johnson

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

DoubleLeo — Wed, 06 Jul 2022 17:29:57 GMT

I too am experiencing this issue. I build my initial models as multi body part files and then export each solid into parts / sub-assemblies via "make components" in the "manage" tab. When exporting parts from my muti body part file I make sure that the "link sheet metal styles" box is not checked. I have prepared a number of different sheet metal template files that already have the proper material type and thickness integrated into the sheet metal defaults; I select from this list of prepared sheet metal templates when exporting my parts from my multi body parent file.

Initially this works great, however, I have noticed that there are certain actions that seem to cause Inventor to revert all my sheet metal defaults in the files exported from my multi body parent file back to all default settings. Actions such as exporting my BOM from my top level assembly in excel format. Materials are changed back to 'generic' and thicknesses are set back to '0.120 in'.

I have attached an example for your reference. Hopefully this help in solving this issue.

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

johnsonshiue — Wed, 06 Jul 2022 20:45:32 GMT

Hi! Many thanks for sharing the files! I think I know the behavior you are talking about. It is specific to Sheet Metal MSB workflows. The main reason is that the body thickness cannot be easily altered in the derived part itself. It is still mainly driven from the MSB source part.

At the moment, I have hard time finding the relevant components. Could you walk me through a workflow showing the exact problem?

Thanks again!

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

DoubleLeo — Wed, 06 Jul 2022 23:43:12 GMT

The files I sent you are small in number and pretty simple in terms of number of parts. I am thinking this would be a good example for us to use to troubleshoot this; less variable to nail down.

We could start with any one of the part files with a name that starts with "MB". MB stands for multi-body. Lets pick the "MB SOLID - ROUND BOLLARDS (SHALLOW)" file. This is a standard part file, (not a sheet metal part file), that I use to develop the design. Once the design is finalized I use the "make components" function within the "manage" tab to push parts from this parent file out into sub-assemblies / parts. There are two main windows that come up when using the "make components" function; the first one is where I choose which solids to push out into sub-assemblies and the second window is where I decide which part template to use when pushing out said solids. It is in this second window that I choose which of my many sheet metal part template files to use for each solid. I have already prepared a set of sheet metal part template files ahead of time with the specified material type and material thickness entered and saved within the sheet metal defaults dialog box. This way, all solids that are pushed out from this parent MB solid already have the proper material type and thickness entered into the sheet metal defaults; all I have to do is define A side and produce my flat pattern for any and all plates.

I would like to mention that, due to the fact that each of my sheet metal part templates has a variation in its sheet metal default settings, (material type and thickness), I do get a window popping up when pushing parts out into sub-assemblies that warns me that the document styles are different from the overall inventor library styles. I typically just ignore this and everything is fine.

The fact that my sheet metal styles were overridden is a new development; one that has not happened to me after years of using inventor. I hope that this is enough of an explanation for you to troubleshoot this issue.

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

DoubleLeo — Wed, 06 Jul 2022 23:46:08 GMT

If you are simply having trouble figuring out which files control which files:

MB Solid - ROUND BOLLARDS (SHALLOW) controls all the parts in assembly SHLW-BLRD-A. From there you should be able to connect the dots down to the part level.

Re: Sheet metal style still linked after "Link sheet metal styles" is unchecked

johnsonshiue — Thu, 07 Jul 2022 20:21:46 GMT

Hi! Many thanks for the additional detail! I think I may have a theory on why it behaves this way. This is a case of style naming collision. It seems to me that the "Default" sheet metal rule has different thickness values in different sheet metal template files. If my suspicion is true, there will be problems.

It is always better to have unique names. If I were you, I would name the rule with its unique thickness value like "0.375in" or "Gauge 0.375." Make sure you set it as the default rule (Sheet Metal -> Sheet Metal Defaults) in the sheet metal template file. In this way, the style will be different than the "Default" in the style library.

The warning about style conflict actually denotes the problem. You dismiss the warning, meaning the library "Default" overrides the template "Default." As a result, the settings are all overridden.

As I mentioned above, the quickest way to avoid the problem is to rename the rules. Please try it out and see if it works better for you.

Thanks again!