What is an Inverted Mesh Element?

[ryandias]

I am new to (Stress/Mechanical) FEA. I am trying to use Comsol Multiphysics to show stress's on a plastic connector.

My past experience is with CF Design (cfd) and I am not finding it any help trying to use the mechanical software.

I keep getting an Inverted Mesh error. What exactly does this mean? What sort of geometry would cause such errors (what should I change in the CAD, or is it a matter of changing settings)?

Earlier post in the wrong section

http://www.eng-tips.com/viewthread.cfm?qid=229673&page=1

 

[rstupplebeen]

My guess is that you have an element inside out. A 2D example would be the nodes of a square could also make an hourglass shape. More details about what software you are using would help provide a better answer. Hope this helps.

Rob

 

[johnhors]

All FE solvers that I am aware of require that the nodes of an element are presented in a particular order. Reverse that order, then in 2D the solver may report a negative area element and in 3D a negative volume. Jumble up the order and a variety of element quality errors may be reported, Abaqus will actually ask you to check the element node numbering order.

Having said that, I expect that very few users will be building data files by hand, thus with a pre-processor to generate the mesh this kind of problem should never happen! But occasionally when geometry is imported from CAD that is particularly nasty, screw ups can occur and some pre-processors can generate illegal elements giving rise to these error messages.

 

[ryandias]

my understanding after researching some more is that as the model "deflects" under load, it can cause some mesh's to invert. Comsol gives me the option to allow remeshing during a simulation, and this is what I am trying to do now.

Are the Pre-Processor's you are using specific to the program? or do they work for any simulation software?

 

[spongebob007]

What I suspect you are referring to is an inverted Jacobian error. In very simple terms, it means your mesh has elements that are distorted. They may either be distorted due to the meshing operation or they may become distorted during the solution as a result of very large deflections in your model.

Essentially the Jacobian operator relates the natural coordinate derivatives to the local (or global) coordinate derivatives for an isoparametric element. So you can think of it as a mapping between coordinate systems.

d/dr=J*d/dx where r is the natural coordinate. We can also say that d/dx=(J^-1)*d/dr. In order for J^-1 to exists, there needs to be a one to one mapping between the coordinate systems for an element. If an element is highly distorted (for example large interior angles) this one to one mapping does not exist. For highly distorted elements J is singluar and therefore J^-1 does not exist.

 

[ryandias]

Spongebob007 - I think you're correct. My coworker found me a document that illustrates the inverted mesh error, and how to "remesh" during the simulation.

I made the changes, and ran it. It seemed like it was working (took a long time) and then crashed with ... "inverted mesh"!

I'll try again. Perhaps I can change how I apply my forces.

 

[spongebob007]

Natural coordiantes can be thought of as a coordinate system that is internal to the element and independent of the global coordinates.

For example, consider a two node truss element of length L positioned along the global X axis. The global corrdinates of the nodes would be x1 and x2 respectively. The natural coordinates of the two nodes would be -1 and 1 respectively.

 

[spongebob007]

What kind of simulation are you trying to do? For linear, small defelction types problem, I have never heard of a case of the mesh becoming distorted under the actions of the loads. If you are running a linear analysis and getting this error, chances are it is your original mesh that is distorted. I am not familiar with Comsol, but most FEA preprocessors have a mesh quality checking feature that will highlight warped elements in the mesh. You can run a mesh quality check to see if this is the case. If you find distorted elements you can try remeshing with a finer mesh density, applying local mesh controls, or modifying the CAD geometry to better accomidate the mesh. Some codes also have "auto fix" features that attempt to fix bad elements.


Sometimes you can force your model to run by turning off the automatic mesh checking. Again, I am speaking in generic terms becasue I don't know if your program has these features.

 

[ryandias]

My company builds automotive electronics. We have a plastic connector assembly that is attached to an aluminum housing using 4 spring pins. These pins hold the connector against a flat surround which compresses an O-ring creating a water proof seal.

The spring pins also must support against someone tugging on the connectors (150 N).

My simulation has to correlate the existing connector with a new suppliers "cored" version of said connector. I am trying to confirm that the strength of the unit has not diminished.


On a side note, I have been "cutting" up my model into 4 separate parts, and running the simulations separately. I hate doing this, because I think it's important to keep them as one piece so that the interaction is evident.

Anyways, Thanks again! I'll keep updating as I progress.

 

[jte]

ryandias-

One issue I could see with a CFD-FEA crossover is that you may be using too fine of a mesh. Structural meshes can be much more coarse than you may be used to seeing in the CFD arena. The connector you're modeling just doesn't seem big enough to require so many elements that you'd have to break the model into four parts just to run it in a reasonable amount of time. Assuming that you are using a solid model, you could start with a mesh size no smaller than the thickness of the part and see if your model runs in a reasonable amount of time. If it runs, at least you know you've worked out the bugs in the geometry and boundary conditions. Then refine the mesh until you don't see substantial changes in results.

jt

 

[btrueblood]

Tried to post this yesterday, but it didn't come thru.

"My simulation has to correlate the existing connector with a new suppliers "cored" version of said connector."

Ryandias - if the supplier gave you the geometry file, and you converted it from a non-native source (for Comsol) it may be the root of your problem. It is quite possible that the "core" was created using a mesh having a different "handedness" than the original file, resulting in the Jacobian errors you are seeing. I was able to create such files using an early version of an Autocad product, where I was doing a "boolean" subtraction operation to core out a part; the resulting file had all kinds of nasty things happening, until I abandoned that approach.

You should try to build the model file from scratch, within the COMSOL environment, and see if it doesn't run a bit better.

 

[ryandias]

That is really not an option. Comsol's geometry/cad is much too slow to try and recreate this connector. I had originally tried to build it in Comsol, but I think I'm just wasting more time.

This morning, I ran some simulations on our existing connector (4 partial simulations), with no inverted mesh errors. This is from native files, but is input into Comsol using parasolid files. The supplier files I input into comsol were converted from STEP to Parasolid, and then input.

I am going to try and run a simulation on the whole connector this afternoon sometime, to see if it causes errors, or works fine as with the individual sections.

 

[spongebob007]

Have you tried to see exactly which elements are giving you problems?

 

[ryandias]

Ran the simulation on the whole connector (less detailed on), and it had the same inverted mesh error. It did give data, but I am not sure how reliable the data is.

The inverted elements seem to be on a flat section, in the middle (no features).

 

[btrueblood]

"The inverted elements seem to be on a flat section, in the middle (no features). "

Next to the wall/forming the wall of the cored part of the model? If so, bingo for my prior post - the model was constructed without keeping the same coordinate system "handedness" from parent to child, probably by constructing the core as a boolean subtract operation. The vendor's files are worthless to you.

 

[btrueblood]

"That is really not an option. Comsol's geometry/cad is much too slow to try and recreate this connector. I had originally tried to build it in Comsol, but I think I'm just wasting more time.

This morning, I ran some simulations on our existing connector (4 partial simulations), with no inverted mesh errors. This is from native files, but is input into Comsol using parasolid files. The supplier files I input into comsol were converted from STEP to Parasolid, and then input.
"



It sounds like you have not modelled the cored connector in ANY modelling software? Could you not model it (the cored part) fairly quickly in SolidWorks or Inventor, or whatever was used to generate the original connector parasolid file? Then import the parasolid to Comsol and mesh from there...

 

[ryandias]

I recieved the Cored model in STEP, but had to stitch quite a bit to get a solid.

Our system is Solid Edge ST.

I stitched up the broken surface model and got a solid. Then output a parasolid and imported to Comsol.

"without keeping the same coordinate system "handedness" from parent to child, probably by constructing the core as a boolean subtract operation. The vendor's files are worthless to you."

Entertaining this. Can you explain this in "wife" terms? I am not catching why boolean operations would affect the quality of the model? After it is output to STEP isn't it completely dumb anyway?

 

[spongebob007]

I am also not sure how boolean operations can lead to meshing errors.

 

[johnhors]

SpongeBob - They don't!

Ryandias - STEP (and IGES) whilst providing a perfectly good BREP (boundary representation) of a solid volume are as you say "dumb" - they don't contain any information relating to boolean operations or a CSG (constructive solid geometry) tree. Any pre-processor will import the geometry and if necessary topologically "adjust" the face definitions such that all face surface normals will either all go into the volume or all go outwards. They have to be consistent, only then can the model be correctly meshed. I would find it very hard to believe that any meshing software could be adversely influenced by "handedness" within the original CAD system.

 

[btrueblood]

"Any pre-processor will import the geometry and if necessary topologically "adjust" the face definitions such that all face surface normals will either all go into the volume or all go outwards. "

I've seen it happen, especially when translations are made from surface models to solid models, and have had problems in particular when using boolean subtractions to "core" a parent solid. IMO, there are likely areas within (beneath) the stitched surfaces that did not get treated by the preprocessor.

But, we clearly have experts on preprocessors here (and I am definitely not), so I will respectfully bow out of this discussion. Good luck, Ryandias.