Meshing error depending from orientation of the same model

Rino_aic

Why if Do we try to meshing same model (changed just the orientation) we have error in just one? How could I solve? Thanks

disla

I don't have any issue ?¿?
Just some elements of difference. (Netgen 6).

Rino_aic

Sorry... wrong file

disla

Try to install Gmsh and link it with MECWAY.
Regarding Netgen, I normally set the elements per curve and elements per edge to 0.01.
I saw it a long time ago in a post at this forum and it has a lot of sense.
If you have two sides of different length together and you request the same number of elements per edge, it is impossible to get a conformal mesh. Leave those numbers close to cero if you are looking for a conformal mesh. It works fine.




For some reason this step takes more time than usual to mesh. (4 min). Be patience.

Victor

As @disla said, use Gmsh. It solves a lot of mysterious meshing failures. The only reason it's not the default or even the only mesher is that it's free software with a capital "f" so it doesn't want Mecway peeing in its sandpit.

prop_design

Your Serb_A.stp file meshed fine in the current version of Netgen. This is from the Netgen website. It only took about 29 seconds on a modest laptop. I'm not sure which file is the one that wouldn't mesh for you though.

The versions of Netgen built in to Mecway have problems. With the version from their website you also get a quality plot for solid models and parallel processing. The fine settings usually work good for me. I experiment with the max and min element size. It worked for 10 and .1. It also worked for 10 and 0. Sometimes 0 as the min size can cause it to crash. Your model didn't have that problem though.

prop_design

I ran a quick test on the vol file, just to make sure the mesh was valid. I don't know your loads, materials, etc... However, I did notice those tabs at the top have re-entrant corners. This will cause the FEA results to be off, in those areas. You would need to add fillets or chamfers, to avoid that problem.

Rino_aic

Thank you Guys...

The problems I'm encountering with MECWAY are not only related to meshing, but in very long attempts to analyze FEA that return errors or with solutions that do not converge.
In the attached example I'm trying to find a configuration that returns a solution. This is a real application of the fixing of an LPG tank installed under the trunk of a vehicle, in which the tightness of the bolts (preloaded with 15kN), the tearing of the trunk sheet (plate) and the fixing points on the thank must be validated. (Nuts are welded under "U" profile welded on the thank)
I have simplified the model as much as possible, eliminating the whasers and simplifing the sheet metal of the trunk.
The verification must consider that in the event of a crash the tank is subjected to a force of inertia of 20g, (a force of about 15kN applied in the center of gravity of the tank, which we make approximately coincide with the geometric center of gravity).
Could you help me understand how to find a good setup in MECWAY FEA for this test ??

https://we.tl/t-6OsIfma09v (to download all files)

disla

There are many things going on there. I would split the problem and proceed by steps.

I would suggest you try to find a convergent solution first with linear elements on a reduced model (See pic). It contains most of the details to be solved and each run will be much faster. Increase the density of the lifting lug to match 1/5 of the whole tank mass if you want.

Once you understand the problem and make all the contacts work, I would include the whole model just up to the lifting lugs. (lighter model). Then, you will have to deal with how to apply the BC on the supporting system (Beam ends and plate). Don't worry about the tank yet. Increase the density of the lifting lugs to match 1/5 of the whole tank mass each.

Once the bolts and supporting system is verified (flat plate seems the weakest ), you could include the tank to finally check the lugs and head area. (Check the mesh problem detected by Prop_design and don’t forget to re-establish the lifting lugs density).

Note: LPG will be compressed around 20 Barg so there are pre-existing stresses on the tank. Inertia should consider Tank self weight + its content.

Rino_aic

Thank you disla


Absolutely yes, I need for an initial linear solution to then transfer the macro-results to the single details to deepen with the non-linear checks. The tank is not the subject of the analysis, and an LGP tank is subject to a maximum test pressure of 3 bar, so I could simulate it in the model using a simple disk that connects only the fixing points with a long central element on which to apply the force of inertia.
My task is also quite simple, it is only a question of verifying if any failures occur and not of finding a suitable solution. The vehicles are existing and cannot be modified.

disla

Hi
I would solve one of the bolts with its contacts first (master/slave, stiffness values, tie or elastic,...) Once it works, then i would go to the full model with more confidence and not wasting computational time.
I have done a quick first run and needed 5 contacts with two of them not easy (spacers through the holes) . Some elements were bad with negative Jacobian. I would build five of those nice hex bolts that John explained how to do. The automatic meshing is not providing good VM (peaks of 1404 MPa).
If you visualize your system as a Vessel with legs under a strong horizontal action you could advance where the hot spots will be as it is not brazed.(1mm plate as "foundation")

Note: GLP at 3 Barg is a gas ?¿?.I know GLP from industrial installations not automotive and it is stored liquiefied tipically between 14 Barg and 20 Barg ambient temperature. Automotive probably less but still should be liquid (10-12 barg). I would check that with the supplier.

Rino_aic

Hi disla,

Could you attach your liml file?.
Thanks

disla

This is a 3 min run very raw just valid to check contacts and estimate parameters.

https://we.tl/t-CAhFphCTiJ

Rino_aic

Thank you again disla