What is an Inverted Mesh Element?
What is an Inverted Mesh Element?
(OP)
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/viewth read.cfm?q id=229673& amp;page=1
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





RE: What is an Inverted Mesh Element?
Rob
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
Are the Pre-Processor's you are using specific to the program? or do they work for any simulation software?
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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
RE: What is an Inverted Mesh Element?
"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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
RE: What is an Inverted Mesh Element?
The inverted elements seem to be on a flat section, in the middle (no features).
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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...
RE: What is an Inverted Mesh Element?
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?
RE: What is an Inverted Mesh Element?
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
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.
RE: What is an Inverted Mesh Element?
If your model is undergoing extremely large defelctions then you might need to remesh the model at different solution steps.
One example of this problem would be metal forging/forming analysis. The deformed shape is so different than the original shape that the elemnents will distort during the solution phase. Is it possible this could happen during a non-linear simulation of an elastomer? I don't have much experience with FEA of rubber parts.
RE: What is an Inverted Mesh Element?
Materials properties are as on the PBT gf 30 spec sheet.
Force is as in the image.
[IMG]http
RE: What is an Inverted Mesh Element?
Your overall element quality will be a function of how robust the mesher is that you are using. I find that for some codes, the "auto mesh" functionality often chooses element sizes that are too large for the geometry. The mesher can compound this problem by trying to fit elements of all the same size to the geometry. Some codes have smart meshers that will identify small features and adjust mesh sizes and element size transitions accordingly.
You might have to resort to using local mesh controls to get a good quality mesh. Sometimes splitting up the solid into multiple bodies is what you are going to have to do. If possible, defeature the geometry. Remove all small features that you feel don't contribute to the overall response of the model. This is easier said than done when you are working with imported geometry. Many of the higher end preprocessors can delete surfaces and heal imported geometry even without model history.
RE: What is an Inverted Mesh Element?
So this brings up another question then. What is an appropriate mesh.
Is the attached mesh ok, or is this causing my problems?
there are some larger tetrahedrals in the middle areas, and very fine ones near the holes.
I have tried refining the mesh, and only resulted in longer run/fail times.