Large assemblies pre processing 3

[FEAsolver]

I do have a large assembly where initially i used solid element to mesh. Recently I end up using shell elements (model has over 100 parts/plates on it) but I get different error messages such as flexibility matrix singular or excessive deflection. Could someone please advise on how to check my model to find the root cause (I use ALGOR). Is it due to constraint or large forces or ...? Thanks

 

[GBor]

You may want to post this in the Algor Forum (forum810), but it is difficult to know what to suggest without a little more information. Did you auto-mesh? If so, did the mesher indicate any problems? Is this problem linear? Or do you have contact? Would it be prudent to have some shells and some bricks? Could you simplify the problem with other element types in places where you aren't as interested? Or could you run a global, coarse model, and the refine a local model?

It sounds like the model isn't properly "stitched" together. Did you run any of the geometry clean-up routines such as "global snap", "delete short", "delete unconnected"?

Since you are using "shell" elements, I assume you are non-linear. Do you have a machine that can run a non-linear, 100 part problem? This doesn't sound like a trivial problem. Have you contacted Algor?

What version of Algor are you running?

Sorry there are many questions and no answers, but a little more information will likely go a long way.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[FEAsolver]

Thanks Mr. Borowski,
to answer to your questions, yes I auto-mesh the model however i refined mesh in the area of interest. The mesher did not indicate any problem nor warnings. This is a static stress with linear material problem. the parts assumed to be in full contact (bonded). I tried having some brick (solid) elements where i had constraints and loadings and use shell elements for the rest of the structure but still getting "felixibility matrix singular" error. I changed the mesh size and still no results. i changed the constraint and fixed the nodes and getting results but excessive deflections (100,000 + inches !). Algor's common structural analysis error messages suggest that the felixibility matrix singular error should followed by the element# and node# but i don't get any of them. I contacted ALGOR and recommended to check the model (that is my question how to check the model and from where/what to start?)
The machine can handle 100+ parts and running ALGOR Release 18.1.
I haven't done any clean up on model but could you please advise on how to do that is it something in ALGOR or i should do it in CAD?
Thanks Again.

 

[prost]

I don't know anything about ALGOR; however, the unspecific advice "check the model" seems to be something they teach product support people to say when they can't think of anything else to do, as this appears to be common advice from a couple of FEA S/W companies I have encountered.

As far as checking the model, you say you refined the mesh in the area of interest. Red flags that pop up are 1) "materials not assigned to ALL elements" though that should give you an error such as 'element stiffness matrix for element XX could not be computed' and 2) elements not connected as you think they should be--there might be free edges and/or surfaces internal to the mesh outer surfaces, and you didn't mean to put a crack there at the internal free edges.

The last red flag is the use of several kinds of elements. There are almost always compatibility problems between elements of different formulations. For instance, connecting a shell with a solid (hexahedral, for example) points to a possible compatibility problem where the shell connects to the solid, because the displacement fields (that is, the allowable degrees of freedom) of the shells and the solids are not the same. Normally great care is taken to make sure that there is compabiliity by using special functions at the interfaces; personally I wouldn't trust that totally until I ran a few test cases in which you use shells and hexahedra in one mesh, and replace the shells with more hexahedra in another mesh; compare the results. Of course you would be using a small subset of the overall large structure you are trying to analyze.

 

[FEAsolver]

Thanks for the comments PROST,
Checking the model as you mentioned for a simple structure is very easy but my problem is that the structure consist of about 150 parts (all same material though) and weight about 20,000 lbs. i checked the model in CAD for any interference of the parts and so far no issue. currently i use all shell element in the model (no more solid) and all materials as well as element definition (Isotropic + thickness) were defined. my problem is to find the reason of getting the error message "felixibility matrix singular" in my analysis. The common following practices were all checked:
incorrect contact
changing mesh size
over-constraint
under-constraint
do you know any back door based on your experience regardless of the FEA software to check for the validity of the 3D model?
thanks,.

 

[johnhors]

FEAsolver

One very useful technique to identify under constrained parts is to run a natural frequency analysis. Modes with a zero or very near zero frequency indicate rigid body motion and thus an under restrained part of the model, the associated mode shape will be the rigid movement of the offending part or parts.

"felixibility matrix singular" makes no sense ! Are you sure that it says this, as an under restrained model has a singular "stiffness" matrix. The flexibility matrix is the inverse of the stiffness martrix, and thus cannot exist if the stiffness matrix is singular.

 

[GBor]

Nice one, John.

Yes, FEASolver, run the frequency analysis, but I have to question your modeling technique if you have 150 parts of the same material bonded together and you are meshing them separately. I would suggest that you merge all or most of the parts in your CAD model before exporting them to any FEA software. Everyone believes their "software of choice" can mesh anything, but to match the mesh of 150 parts is difficult. Merging the model and exporting a single solid will make this easier for the mesher.

Is there some reason why you need all 150 parts in your FEA model? If this is a linear static problem, seems like a single part should do.

What CAD modeler are you using? The difference between a CAD model and an FEA model is often huge. You may not be getting any interference, but are they in intimate contact? If not or if they are, but at a larger tolerance than the gap that the FEA software will catch, Algor may not think you are in contact and, therefore, may not be matching the mesh. If the mesh is lined up and the nodes coincident, the processor won't recognize the bond.

The model clean-up is under "Tools: CAD Preparation", I think.

 

[GBor]

Reading my own post, I'm confused!

I meant to say that if there is a gap between parts in your CAD model, then Algor will not try to match the mesh of adjacent parts. If the tolerance in your CAD model is 1e-5 and Algor is reading double precision accuracy of 1e-15, Algor may not recognize two parts that are 1e-8 as being "in contact", so the mesh will not match and parts will be detached.

This will become obvious running the frequency analysis as johnhors suggested. You will have entire parts "flying off in to space".

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[smurgie]

Hi FEAsolver,


Garland, prost and John all gave excellent advice. If you still need additional assistance, I strongly urge you to contact ALGOR Technical Support.

Sam Murgie
Manager, Software Development
ALGOR, Inc.

 

[FEAsolver]

Dear Sam,
i should admire ALGOR for the excellent software and the ease of work with it, but i believe it is not a software related issue i am trying to solve a concept in my model. ALGOR already offered me to send the model to be analyized (thanks a lot for the offer again) but as i mentioned we try to resolve the similar issues and learn something from it and share the experience.
Thanks all.

P.S. to GBor
the clean up you referring to is on FEA editor under Geometry -> Utilities and ....

 

[GBor]

Sorry, FEASolver...I'm not at my desk. Minor flashback to Superdraw III where it is under Tools. Thanks for clarifying.

 

[rcorces]

I would like to offer some advice on how you may be able to find the problem area when you get the flexibility matrix singular message.
After the run error message,
1. Click on report and then summary. Then go to bottom of file. There you will see the location where the error occurred and the very last element that was input
for example:
6241 22049 22115 22116 22116 0 7 5.000E-02 0.000E+00 0.000E+00
error: flexibility matrix singular
Error.
2. Then go to the results tab at the bottom of the parts window and then select top menu INQUIRE/ELEMENT Information
3. A window opens up. Input the part number and element number from step 1 above. You will have to try different part no.s until you see the element with correct node numbers. This could be very difficult and tedius if you have many parts in the model.
4. look at the model. The element outline will be hilighted. But, you may have to hide some parts in order to get a good view.

Good Luck. Ron Corces, P.E.

 

[johnhors]

Hi Ron,

Sorry to have to harp on about this, I've never used Algor but from a purely mathematical point of view a singular flexibility matrix is simply an impossibilty ! I'm sure Algor really means stiffness matrix.

If as your post suggests that the error message is pointing to a specific element, then with solids a very poorly shaped element may have negative volume and/or bad jacobian ratios, but this should not be a show stopper, most solvers stop only because element quality fails some criteria test, and can be forced to continue (like Nastran with tetraar statement) by resetting the acceptable limits. However the OP says he is now using shell elements, which should rule out poor element shapes as being the problem!!!

I believe the OP should forward his model to Algor.

 

[cbrn]

Hi,
probably my comment sounds a bit obvious and I apologize in advance if I unadvertedly missed some point in the previous discussion, but what hit me was when the O.P. says he shifted from previous solid mesh to the current all-shells mesh. By doing this , he has gained 3 more DOFs at each node, since shells nodal DOFs are 3 translations and 3 rotations. By consequence, the original restraints may not be sufficient any more, I mean that probably some of the rotations, if not all the rotations, are not "globally" restrained.
I 100% agree with the modal analysis system as a way to determine the existence of rigid body motions.

Regards

 

[freiFEM]

FEA Solver,

May be my experience with NASTRAN in a simillar case would be helpful to you. I have no experience with ALGOR. I have also faced simillar problem when i was working with large number of parts in a single assembled part. When i have gone through "f06" file, i found that, there are some elements which were exceeded the limits of tolerance angles and related to this DOF is also excessive. As a test i simply removed those elements, then it was fine and i had no problem with analysis. But here the main thing i should mention is, i have generated "automesh", and obviously "tet" elements are default. So if you remove them it would not be a problem. But you have mentioned you shifted from solid elements to shell elements. In your case the reason could be lie in the area of excessive DOF i.e as "cbrn" said, shell element has 3 more DOF than solid. If you would not shift from solid to shell elements, i would say, your problem also will be solved in the same manner that i have done.

good luck,
Tobias

 

[rcorces]

John, I agree with everything you have said. I was merely trying to help find the element where the error occured. I had the same problem yesterday and I am still trying to resolve it. Some times the error message is not precise. So, as you said, it is probably associated with stiffness matrix.

I have one additional helpful hint. In my previous message, the listing for material no. (which was 7 in my example) should also be the part no. This should simplify locating the element.

Ron Corces

 

[EdR]

FEAsolver:

I admit I did not read all the posts in detail but your comment that you are getting a deflection of (100,000+) indicates an unconstrained model......Look for unconstrained dof (or parts) that allow rigid body motion to occur...

Ed.R.

 

[hansm2]

Run a normal modes analysis with all constraints removed. You should have 6 rigid modes followed by flexible modes. More than 6 rigid modes means you have mechanisms. You will see where they are from the mode shapes. Output strain energy and that will help show bad elements in the rigid mode shapes. I have not read all the posts so this may ne redundant.