Error when trying to shell a part

[zceme76]

Hello community,

When trying to shell a part i get the error: the attempted shell operation was unable to solve for a vertex....etc. i have attached the problem part file, of which the drawing is a fairly complicated frame (a chassis concept for a 3 wheeled race car i am designing)

How the part was made:

It was created in an assembly using the frame generator tool and then converted to part file using the shrinkwrap feature. When using the shrinkwrap command, i selected: single solid body merging out seams between planar faces, All hole patching, break link, and remove all internal voids. and then when trying to shell i get the error message when selecting a wall thickness of 2mm.

i cant understand why the shell feature does not work as i have successfully shelled a very similar part file (with only slight differences in geometry from the file attached in the same way as what i am trying to do with this part). i can provide this part file upon request or the assembly file from which either was created. i need to shell the component in this way so that i can run accurate FEA (stress analysis) for crash simulations on it

Any help would be very much appreciated, thanks

I am using inventor 2013 (64bit OS)

[jakefowler · Accepted solution]

Hi,

Many thanks for posting this problem! I've taken a look at your operation, and it appears that there is just some geometry on this particular model that is causing difficulties for the Shell computation (i.e. I do not believe this to be a general limitation of this workflow). I've logged the failure to shell this model as a defect with the development team (Defect ID 1460070, should you need this for future reference) so that we can try to get this case working for a future release.

I've managed to come up with a workaround for this model (IPT attached - End of Part marker is rolled-up to reduce file size): this involved omitting problematic faces from the model before shelling, then using the Thicken and Delete Face tools to hollow-out and attach these segments separately.

Here's the full process I followed:

1. To find the region(s) that are problematic for shelling, I made a sheet copy of the model, and used the Thicken tool to 'simulate' the Shell operation face-by-face. By continually adding faces to my Thicken feature, and noting where they failed, I narrowed-down the problematic regions to a few model faces.
2. Starting afresh, I made sheet copies of these problematic model faces, using the Offset surface tool with an offset value of 0.
3. I then used the Delete Face tool, with Heal enabled, to remove the problematic portions from the solid model, leaving me with just a solid shellable part and a set of separate sheets. 
4. I used a 2mm Shell to hollow-out the main solid, then performed 2mm Thicken operations on the sheets to turn these into hollow tubes of the same thickness.
5. The only remaining task was to clean-up the interfaces between the thickened tubes and the main shell. Due to the workaround used, these tubes did not hollow-through to the main shell, and the interfacing model faces did not meet up nicely, leaving some small undesirable voids. I used Delete Face with Heal to create the hollow-throughs, and to tidy-up the interfaces (careful attention was needed here, to make sure all undesirable voids were deleted).

I made this sound complicated, but hopefully you can see from the IPT that it's not that bad :). The aim of giving a lengthy explanation here was to hopefully offer some tips that might be useful if you encounter a similar problem in the future.

I hope this has helped you get around this particular issue. If you encounter problems on an similar parts in the future, please don't hesitate to post them here or email them to myself (at jake.fowler @ autodesk.com), as this kind of data is very useful in helping us improve Inventor for future releases.

Many thanks!

Jake

[zceme76]

Hi Jake,

Many thanks, i have followed your procedure and had a go myself with successful results, so should be able to deal with the issue should the problem arise again.

Again thanks for your help

Dan

[Sledge_Hammer]

I'm also having a problem trying to shell a part getting the same error message "unable to solve for a vertex".

And this one gives me an error message saying "unable to solve for an edge."  

I'm trying to shell both of these with a wall thickness of .03125.  Any help is greatly appreciated...

[JDMather]

Shower Bench -

Have you installed all Service Packs for 2011?

Sketch1 is placed at the origin, but not constrained to the origin?

Are you aware that you can combine multiple fillets of the same size (and even if not the same size) in a single Fillet feature?

Extrusion 3 and 4 are confusing to me.

If you Delete Face the larger faces - there are some slender faces left that I would expect to give trouble.

Downtube -

Sketch1 is placed at origin but not constrained to origin?

I would expect trouble in the areas of Fillets 53 and 54.  (especially Fillet53)

I would expect trouble in the area of Extrusion 22 as well.  Not sure I understand the logic.

If this was my part I would start over with a new attempt using what I learned from this attempt.

[Sledge_Hammer]

Have you installed all Service Packs for 2011?  Yes.

Sketch1 is placed at the origin, but not constrained to the origin?  Before we go any further you need to understand that I have only a basic understanding of how to use this software.  Inventor does not have a large market share so the only place I could find in my state that teaches it wanted $10,000 and a year program to do so.  I opted to hire a student to tutor me in the use of the software until such time as I felt I was proficient enough to use it.  So now you have a solid background in where I'm coming from and what knowledge I have, or not, relating to this software and your vague and ambiguous (to me) responses.

So how does one "constrain to the origin" and why doesn't the software do it automatically?

Are you aware that you can combine multiple fillets of the same size (and even if not the same size) in a single Fillet feature?  Yes and no.  Sometimes I combine several fillets into one feature and other times when I try to do so I get an error message and have to go back and find the problem area and omit that from the string of fillets and handle it individually.  

Extrusion 3 and 4 are confusing to me.

If you Delete Face the larger faces - there are some slender faces left that I would expect to give trouble.  Great.  I have no idea what this means so your comment is meaningless to me.  What does this mean to a layman user?

Downtube -

Sketch1 is placed at origin but not constrained to origin?  This is rediculous.  It should be automatically constrained to the origin!  Why would it NOT be constrained to the origin?  Why would the imbiciles that create this software allow this?

I would expect trouble in the areas of Fillets 53 and 54.  (especially Fillet53)  Funny.  I wasn't expecting to have trouble.  I was expecting the software to understand what I was trying to do, which was blend that loft into the downtube.  It didn't.  So I tried to make a series of fillets to blend it and that was the result.  Operator error?  Apparently, but wouldn't it be nice and wouldn't it be much more user friendly if the software was able to recognize this attempt to blend the loft and do it automatically?  You see this is a common problem with software; it's made by introvert programmers that cannot understand how to communicate to people that do not operate in their programmer mentality.  An excellent example of this is the "Project Geometry" command.  An exceedingly stupid name for this command.  A name of "Project Edges" is vastly superior to the "Project Geometry" name because that's what this command does; project edges!  See the difference?

Instead of getting an error message that says "cannot solve for vertex," wouldn't it nice if the software gave me a promt that said "there's a problem here" and highlights the problem area!  Talk about a lack of logic! 

I would expect trouble in the area of Extrusion 22 as well.  Not sure I understand the logic.  Excellent.  We're both on the same page then.  You don't understand what?  Because I don't understand what you don't understand.

If this was my part I would start over with a new attempt using what I learned from this attempt.  Funny.  I haven't learned ANYTHING yet! And BTW, I did start over and the result is what you see, but in the previous version I tried to loft to the downtube without fillets 25 & 26 with just straight edges and the result was even worse.

So you see what I'm trying to do.  Can you explain what I need to do in layman's terms or can you get someone else in here that can? 

[JDMather]

I tried to walk you step-by-step how to create a part a couple of years ago - but you never responded back.  What happened?

http://forums.autodesk.com/t5/inventor-general-discussion/drawing-a-compound-curve/m-p/3000956#M4005...

From that thread -

Create this sketch and then attach your file here.
(Note the R6 fillet between the lines - this fillet can be any size, but is required.)

As I walk you through this I am going to recommend that you read this document - http://home.pct.edu/~jmather/skillsusa%20university.pdf

If you had continued that discussion we would have discovered that Inventor does automatically constraint to the origin - when set up correctly. 

You will probably want to become familiar with Face Fillets in addition to Edge Fillets.

It probably would have been best to start a new thread for your question as each Shell problem is unique - and this thread has already been marked as problem Solved.

[Sledge_Hammer]

Ok I'll move this to a new thread so we can continue to beat my head against the wall there...