Continious Crashes when applying a bend.

[ENRAD]

Trying to apply a bend in sheet metal, and Invetor crashes immidiatly

[Anonymous]

Your example does not show proper sheet metal technique. You are using part modeling features instead of sheet metal features to make this part.

Instead of Extrusion1, Use the sheet metal Face command.

Instead of the rest of Extrusions, use the sheet metal Flange command.

No need for the Rips at all. Flange can automatically miter the corners.

Have you done the tutorials yet??

This could bave been a 5 minute (or less) part, and easily editable to boot.

[ENRAD]

I am very well aware of that.

However, I am trying to convert existing model imported from SW, without re-do the whole lot.

This is an example what happens when I am applying a bend on an imported SW-part.

But it really does not matter, because Inventor is still crashing completly.

[Anonymous]

You'll not get there with these techniques. here's what I got  in about a minute. See also the attached 2012 part.

[ENRAD]

I Know, but I have a couple of hundred imported parts that will not unfold, due to irregularities in the import (or how the SW-files were created).

The fastest way I found to make them foldable (without redraw the hole project) is to rip up the bends and apply new bends.

But regardles, Inventor is still chrashing when bends are applied.

[Anonymous]

Where are you trying  to place a bend?

[rdyson]

I just tried and second one sent me to CER

Applied first on one of the main face, second on the adjacent edge

[Anonymous]

Model - Bend works here on my modified version of his model. I'd say it's the part. See attached. Is this a sheet metal bend feature you are trying to create?

Using the SM Bend command, I get a crash on the mitered flange edges when selected, but not on the main body. I still state that this is a part error, not an Inventor fault.

Issues here:

The extruded faces touch at the edges. There is no gap.

The bend cannot calculate the the ripped corners.

These errors are due to using improper techniques outside the sheet metal environment.

[Anonymous]

Here's a modification of the original part. Bends work on the main body, flanges work correctly.

Sometimes trying to save time, wastes time.

[ENRAD]

Here is a small video showing what happens.

If I knew what was going on, I can prevent it from happening for the next 100+ parts that needs to be fixed.

THe file was to large for attachement so it is located at www.tlec.se/pub/Inventor.zip

[Anonymous]

I have provided you with a solution. I have nothing more to add.

I explained your crash in a previous post.

[AliceXie]

The problem is that there is no active unfold style in the problem part. Go to Manage > Style Editor > Sheet Metal Unfold to verify it. The unfold style is created and activated when converting the standard part to sheet metal part. So I need to know how can you create a sheet metal part without an active unfold style.

Before I get further information, I can provide another workaround:

1. Go to Manage > Style Editor > Sheet Metal Unfold. Active an unfold style. E.g.. Default_KFactor

2. Change the style thickness to the sheet thickness of your part(e.g.. 1.25mm for the problem part attached in this thread)

Now you should be able to create the bend feature.

[ENRAD]

Dennis, its a workaround, not a solution. Inventor should not chrash regardles.

Anyway, I have decided to re-draw all parts in the assembly, since basically none could be unfolded, probably because of zero inner radious (still wonder why it is converted like this, since I don't have SolidWorks, I cant say if the parts really are designed with zero inner radious, shouldn't though).

Alice, it's simple.

Import sldprt, then convert to sheet metal, thats what I did, set sheet metal defaults, nothing more.

[JDMather]

---

@ENRAD wrote:

(still wonder why it is converted like this, since I don't have SolidWorks, I cant say if the parts really are designed with zero inner radious, shouldn't though).

---

Attach one of the original sldprt files here.

[ENRAD]

Here is the Solidworks file and the corresponding inventor file, as you can se the inventor file is not un-foldable, hense my problems.

[JDMather]

After examining the feature tree in SolidWorks it is apparent that the SWx designer is not experienced with SWx and sheetmetal - check each part very carefully.

[Shiva_Sundaram]

Hi,

I investigated the crash error report and we our tech notes seem to indicate that there is no active unfold style for this part. We are not sure how that happened and we hope to resolve this soon. Is it possible that you have a template which has this problem and no unfold_style has been set? Usually you should get a default style regardless.

One thing you could try as a workaround is to simply activate the default_kfactor unfold style (and I verified this on R2012 and it seems to work and I dont crash)

Steps

1. Open the part

2. Manage tab on the ribbon

2. Styles Editor

3. Expand Sheet Metal Unfold

    **Notice that there is no active style selected (active style would be the one highlighted in bold)

4. Double-click on any unfold style. e.g. Default_KFactor

    ** Default_KFactor would now be highlighted in BOLD

5. Done to exit the dialog

5. Try the bend operation - that should succeed now.

Thanks

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[AliceXie]

I converted the solid works part to Inventor sheet metal part. There is an active unfold style. So I tend to believe that there is something wrong with the template you used which will caused the absence of an active unfold style in the converted part.

However, the converted part do fail to unfold in Inventor. Some addtional information needed for creating flat pattern is not added to the faces in your version of Inventor.

[AliceXie]

I am very curious about how is the part converted like this. I have tried to open solid works file and converted to sheet metal file several times on my Inventor and there is no crash. Would you please check if the "SheetMetalUnfold.xml" and "SheetMetalRules.xml" exists in "C:\Users\Public\Documents\Autodesk\Inventor 2012\Design Data\"(this path is for Vista, Win7 OS, for XP, it is in "C:\Program Files\Autodesk\Inventor 2012\Design Data")? Missing of these XML files in your disk can cause the missing of sheet metal style in the part. 

[ENRAD]

I have:

<SheetMetalRules Version="3">

and

<SheetMetalUnfold Version="3">

In this folder.

The unfold-file has all text in one single row, but I guess it does not matter for an xml-file.

I compared the gcontents with the ones in the Inventor 2011 folder, and they seems to be different