Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Meshing error depending from orientation of the same model
Why if Do we try to meshing same model (changed just the orientation) we have error in just one? How could I solve? Thanks
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
Just some elements of difference. (Netgen 6).
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.
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.
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)
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.
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.
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.
Could you attach your liml file?.
Thanks
https://we.tl/t-CAhFphCTiJ