SHEET METAL // Flat patterns appear as dashed lines in IDW

[chachaman]

Hello everyone,

Can someone tell me why this flat pattern of a sheet  metal part appears with dashed lines in the IDW ? Attached is the part.

Thx in advance !

[mcgyvr]

The whole thing appears as dashed lines to you?

Doesn't for me..

[Anonymous]

When i try to open the provided file I receive a resolve link pop-up. It's for a file "T4_UDM". I skipped this error and attempted to make an IDW but just get an error to resolve the CLPx_2.ipt file before continuing. Sorry i could not help you. I believe your talking about the defulat chain lines that show where the bend is on the flat pattern.

Does it look like these lines?

[chachaman]

Hello,

Here is the part from which it is derived....

[chachaman]

Hello,

Here is the part from which it is derived....

I was not refering to the bend lines...see drawing attached.

[Anonymous]

Did you ever solve this?  We had a random, simple part do this to us this morning and have yet to figure out why or how to fix it.

[mdavis22569]

post your ipt/idw ...

or at least a image of what you're seeing 

[Anonymous]

PDF showing what we see on the drawing and a PNG file showing what Edit View shows us.

We are doing a bunch of brackets similar to this today, this one is the only one acting funny and does so on both machines.

[chachaman]

This happened to me If  part was derived from another part. I solved it by 'refreshing' the derived part. Sometimes when you modify the original part from which you derive from, the changes don't propagate.

Make sure also, you are set with the same thicknesses.

Hope this solves your problem too.

[Anonymous]

Thanks for the update.

This was not a derived part but it was modeled as a flat part with a fold (as several other ones are also.

We re-made the part with sketches for the 2 faces and now it works fine.  Seems like it did want to do some sort of update but we couldn't make it any better.

Anyway, re-making the part was our fix.

[Anonymous · Accepted solution]

Next Time, try this : Go to your sheet metal part > Select the Flat Pattern or the Folded Model, goto Manager > Update > Rebuilt All.

Look at your drawing

Fred Bellekom

Inventor Pro 2016 / Vault Pro 2016

[jeffbohn]

I understand this solves the issue with the dashed lines showing on the idw. but it doesn't address the issue as to why it happens with some flat patterns but not all. I have this issue all the time and have yet to figure out why Inventor does this with some flat patterns but not all.

The solution I have found was to go into the flat pattern, edit flat pattern, select the current axis alignment edge, go back to the folded state and save part. This changes the dashed lines back to the solid lines.

[johnsonshiue]

Hi! The behavior is defective. But, like you said, we don't have a consistent set of steps to reproduce it. Do you have an example to share? Please feel free to send me directly ([email protected]). I will take a look and try to understand the behavior better.

Many thanks!

[DRoam]

Has anyone had any success in tracking down what causes this? It's become more and more frequent for me and it's really slowing down the drawing process.

My sheet metal parts often come from a multibody part, that could be a factor?

Also, does anyone know of an iLogic solution to fix these in bulk? I'm aware that a "Rebuild All" fixes it, but I would prefer for the iLogic to be able to specifically target parts that have this problem rather than rebuilding every single Sheet Metal part. Is there an API property that might indicate when the flat pattern is "sick" like this?

[AdamAG99T]

I've noticed this tends to happen to me when I use Save As to make a new file to modify. It's not consistent but a lot of the time when doing so the original file will have this error occur when I place it into a drawing, while the new file I got from the Save As will work fine. For reference I am currently using inventor 2019 fully updated.

While I don't this this rule does exactly what you want I have made an Ilogic rule to quickly fix a drawing view experiencing this error from within the drawing. You simply select the drawing view and run this rule. There might be a more efficient method to fix it with Ilogic but I've had this working for me for a year or 2 now. 

Try
Dim oDoc As DrawingDocument
oDoc = ThisApplication.ActiveDocument
oDrawView=oDoc.SelectSet(1)
Dim oSheetComp As SheetMetalComponentDefinition
oPartDoc = ThisApplication.Documents.Open(oDrawView.ReferencedDocumentDescriptor.FullDocumentName)
oSheetComp=oPartDoc.ComponentDefinition
oSheetComp.FlatPattern.Edit
oSheetComp.FlatPattern.ExitEdit
oPartDoc.Save
oDoc.Activate
If oDrawView.DisplayTangentEdges = True
	oDrawView.DisplayTangentEdges = False
Else 
	oDrawView.DisplayTangentEdges = True
End If 
oPartDoc.Close
Catch
End Try

[johnsonshiue]

Hi Derek,

I believe this is a bug. I thought it should have been resolved as of the latest updates for 2019 and later. If not, something is still wrong. The reason why the flat pattern is in dashed is that somehow the flat pattern body is considered as bend geometry. This does not make any sense. I recall it could be "resolved" by Rebuild All and then the flat pattern body will be recomputed. Somehow the mistake is corrected.

Many thanks!

[AdamAG99T]

@johnsonshiue I can confirm that it is still happening, I just had a part experience this error a few minutes ago, and I am fully up to date on my inventor 2019 updates with update 2019.4.8. The exact steps I took that resulted in the error were:

- make a new sheet metal part, a simple plate with 1 flange, and create a flat pattern with the file.

- save the part like normal.

- do a Save As to create a copy of this file, as I needed a very similar part with slightly different measurements to the flange.

- save new part again.

- did some miscellaneous work with other part files and used them plus the 2 parts I already mentioned to make a simple assembly.

- saved assembly normally.

-created a new drawing file, specifically a DWG and not a IDW.

-Placed the first part I made as a flat pattern and experienced the error where the entire view is dashed lines.

These steps don't appear to be a reliable method for triggering the error, but as far as I can remember I did not do anything else along the way. As far as I can remember the error also only appears to happen when I used Save As to make a copy of a part to make a similar part with minor changes. In these cases the error always occurs to the original part, not the new copy.

I can resolve the immediate issue easily enough, I have a quick method of simply opening the part, editing the flat pattern, saving the part, then going to the view in the drawing and toggling the Tangent Edges checkbox under the display options tab to refresh the view itself. This is likely functionally identical to the fix you mentioned but at this point I have this method down as muscle memory.

Hopefully you can make some use of this information to find and solve this error. If needed I can send the related files to you as well.

[johnsonshiue]

Hi Adam,

Please send me the files directly [email protected]. I need to see how I can reproduce the behavior persistently.

Many thanks!

[DRoam]

---

@johnsonshiue wrote:

Hi Derek,

I believe this is a bug. I thought it should have been resolved as of the latest updates for 2019 and later. If not, something is still wrong. The reason why the flat pattern is in dashed is that somehow the flat pattern body is considered as bend geometry. This does not make any sense. I recall it could be "resolved" by Rebuild All and then the flat pattern body will be recomputed. Somehow the mistake is corrected.

Many thanks!

---

Hi Johnson, thanks for the additional information, that's good to know. Indeed, it's still present as I'm using Inventor 2020.3 and it still happens regularly. Another thing to note is that in my case, the flat pattern's edges are not using the Bend line style; instead, they're using a hidden-line type style. Through some experimentation with our Object Defaults, I was able to determine that in fact it's using the "Hidden View Edge" object type's layer. So apparently the body is considered as "Hidden View Edge" geometry rather than bend geometry. Also worth noting is the bend lines themselves display correctly (as bend lines). Hopefully that helps in further tracking down newer manifestations of this bug post-2019.

Also, for me, unlike Adam, it's unrelated to "Save As". My sheet metal parts come from a multibody part, and are always created using "Make Components", and there's no Save As anywhere in their history. So "Save As" may be one failure mode, but it's not a requirement.

Lastly, indeed a Rebuild All on the individual Sheet Metal part does correct the issue. However, it has the undesirable side-effect of causing every parent assembly to need an Update.

[carstenandersen]

Hi

We are experiencing this behavior in Inventor 2021.3.1

This occurs when the file set is a "product" of Copy Design in Vault. Not all of our Copy Designs returns this annoying error, but since we use the function a lot - the problem is increasingly annoying. We have never had the error prior to Inventor 2021 and we do app. 95% sheet metal.

Best regards

Carsten