Sheetmetal Adaptivity - Projections

[Anonymous]

Why does a sheetmetal part, in an assembly, only use projected features from the same sheetmetal part? If you project any other part features, those items are locked and not adaptive. How is this useful? What is the logic? How long can this continue to cause errors in the fabrication of parts?

[Sergio.D.Suárez]

Hi, Excuse me if I don't understand you correctly, I have a sheet metal component in an assembly. I edit the sheet from the assembly, then create a sketch and project an edge of another part, even of another sheet.
In order for the projected entity to maintain association with the edge of the part from which it was projected, the following boxes must be previously activated in the application options.

In many cases of dynamic design, associativity is not always sought to create adaptive parts, many times adaptive parts can give problems. But for reasons of practicality, entities can be projected and they will be fixed in space, so we can eliminate the fixed restriction and place a dimension to place it correctly.
I hope I have been clear, and that you can solve your problem quickly. Regards

[Anonymous]

Features projected to a sheet metal part, in an assembly, will be fixed and not "truly" adaptive. This becomes an issue when you expect features to move (adapt) and they do not. This is an ongoing issue with Inventor.

This is a simple part example.

The attached image shows:

1) Yellow ... projected edges of a sheet metal part.

2) Blue .... projected edge of a hole form a mating part. Note that it is fixed.

3) Red .... highlighted, projected edge of a hole form a mating part. Note that it is also fixed.

I would expect all projected edges to be yellow (adaptive) and they are not.

[IgorMir]

Hi Mike;

It is not an Inventor issue, really. I would suggest you review you design practice and avoid using project edges on the assembly level. Use Derive Parts workflow instead and leave assemblies for what they are intended to be used. I.e - for viewing your assembled model - not creating it in there.

Cheers,

Igor.

[johnsonshiue]

Hi! Please check the options Sergio mentioned in his replay (Tools -> App Options -> Assembly). Another two possible causes. 1) You project assembly sketch geometry to a part sketch. 2) You project OccurranceA geometry to OccurrenceB, while both occurrences point to the same ipt file.

Many thanks!

[Anonymous]

Thank you for the reply. The options are set correctly. I only have this issue when a sheet metal part is involved. I never seem to get the feature to be adaptive when linking features in an assembly.

[johnsonshiue]

Hi Mike,

Please share the files with me directly ([email protected]). I should be able to tell where the problem is.

Many thanks!

[Anonymous]

I made a generic assembly to show that this is a repeatable issue.

[johnsonshiue]

Hi Mike,

Many thanks for sharing the files! I took a look and tried it on my machine. I am not seeing the issue. The only explanation I can come up with is like Sergio's post#2. The two checkboxes are unchecked in Tools -> App Options -> Assembly. Could you take a snapshot of the option dialog? I would like to see if the two checkboxes are checked.

Thanks again!

[Anonymous]

Try moving any hole on the Base Block and tell me that that the holes move on the mating part. The Projections are locked and are not adaptive. The sheetmetal parts are not truly adaptive.

By the way, this is the 2019 version. It has been this way as long as I can remember. And, I always use adaptive parts.

[johnsonshiue · Accepted solution]

Hi Mike,

I think I see where the problem is now. This is about the a document setting in the sheet metal part. The reason it cannot be adaptive is because it has been adaptive in another assembly. A part cannot be adaptive in two different assemblies. Here is what you need to do.

Open the sheet metal part or edit it in-place.

Go to Tools -> Doc Settings -> Modeling -> uncheck "Adaptively Used in Assembly."

Now try project the hole edges. Now adaptive will work.

Many thanks!

[Anonymous]

Many thanks. I have been struggling with this for years. This is the first time anyone actually helped me with this issue.

I find it funny that, this is a new part, used in only one assembly and this occurs.

Greatly appreciate your efforts.

[johnsonshiue]

Hi Mike,

I suspect you have check this box in the part template, right? If yes, you should not check the box in the template. When you attempt to project cross-part geometry, Inventor will check if this part is already adaptive within the current assembly. In your case, the part isn't already adaptive within the assembly. Then the next check is to see if it is already adaptive in another assembly (Tools -> Doc Settings -> Modeling -> Adaptively Used in Assembly). In your case, the part will returns positive. As a result, Inventor assumes this part is already adaptive in another assembly and adaptivity will be suppressed.

Many thanks!