Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

**Jan Goebel****Member**- From: Mannheim
- Registered: 2016-04-02
- Posts: 52
- Website

Hello alltogether,

I'm wondering why I am getting different results for Salome Meca compared with other FE-Software by using the same geometry and the same boundary conditions and material properties. If results would deviate by factor 1000, I would assume a scaling problem, as Salome Geom is scaled by meters, but the results deviation is approx. by factor 20. I have scaled the model by factor 1000 in salome geometry module. Also I have tried to use echelle command in Aster module with the same results. Can anybody help ?

Thank you,

Jan

Offline

**mecour****Member**- From: Ostrava (Czech)
- Registered: 2011-04-04
- Posts: 131

Hello,

can you share more information about boundary conditions, because I think that the main problem can be there. Sometime the boundary conditions are not consistent in different softwares.

mecour

Offline

**Jan Goebel****Member**- From: Mannheim
- Registered: 2016-04-02
- Posts: 52
- Website

Hello mecour,

thank you for your help and the quick reply. I have attached two pictures of the boundary conditions, and, according to your hint, changed the constraint under Enforce DOF from LIAISON ENCASTRE to DX=0, DY=0 and DZ = 0, meanwhile the force on the edge is 100 N (Nodal force), but the result remains the same.

What else can be wrong ?

Thank you,

Jan

Offline

**mf****Member**- Registered: 2019-06-18
- Posts: 22

Hello Jan,

your meshes are both quite different. However, I don't think that is the reason for the difference of DEPL.

a common mistake in ParaVis is to view the DEPL_magnitude after having chosen 'result_DEPL' instead of 'result_DEPL_Vector'. What ParaVis does when calculating the 'Magnitude' (which is not present as data in the result file) is taking ALL components of a data structure. So when you choose the Magnitude of:

1.) 'result_DEPL' it calculates the magnitude of DX, DY, DZ, DRX, DRY, DRZ, LAGS_C (present if DEFI_CONTACT), LAGS_F1, LAGS_F2 (both F1 and F2 are present if FROTTEMENT is active) all together. This is a vector with 9 components. It does not just take DX, DY, DZ.

2.) 'result_DEPL_Vector', it calculates what you want: magnitude(DX,DY,DZ). Just activate 'GenerateVectors' and you'll get 'result_DEPL_VECTOR' as data structure. Then choose magnitude.

Be aware that this is the case for all other data structures as well: result_EPSI_NOEU is different to result_EPSI_NOEU_Vector, etc... you get the idea.

I'm not sure this is your problem, but it is a possibility.

Another possibility: Maybe you chose first order elements for the calculation with the other FE-package and second order elements in Salome? First order elements are stiffer, especially under bending loads. For mechanical problems better always choose 2nd order elements. Although the 20-fold difference might be too high for this possibility.

However, if you could post your .comm it would be easier to judge what went wrong.

Cheers,

Mario.

*Last edited by mf (2020-01-10 21:21:12)*

Offline

**Jan Goebel****Member**- From: Mannheim
- Registered: 2016-04-02
- Posts: 52
- Website

Hello Mario,

thank you for your help. It may be, that the results re correct, but maybe they're not properly displayed. However, I tried activating the Vector view as well as activating the tick mark in the left window, same as going through the menu strucure by choosing Filter --> Common --> warp by vector. It neither generated a new field res_DEPL_Vector, nor showed reasonable results. Hence as the main deformation is taking place in y-direction, I choosed to display y-directiopn displacement only, but here also the results are still wrong and approx. by factor 20 too high. I have attached my comm- file, as well as a screenshot from the y- displacement after activating GenerateVectors checkbox.

As for the elementation I have used quadratic elements for both software packages, so I think this may not be the reason for different/ erroneous results. I have attached my comm- file and a plot with GenerateVectors activated, which doesn't differ much from the original plot. I hope that helps...

Thank you,

Jan

Offline

**mf****Member**- Registered: 2019-06-18
- Posts: 22

Hi Jan,

I see. You do not get it, because you do not have a DEFI_CONTACT or DEFI_CONTACT with FROTTEMENT (they would add components to DEPL). It only has 3 components to start with, so technically it already is a 'reslin_DEPL_Vector'-result. Therefor it doesn't do anything. My bad.

Your .comm is pretty straight forward, did you apply the same force nodale as in the other software? In that case the result will be different (meshes are different).

Could you try the same force on that edge in both software packages (dimension = force per length unit) and please do not use nodal forces? In Aster you should use FORCE_ARETE for that purpose. Please be aware that if your meshes are different in both cases, it is quite dangerous to apply nodal forces as they are mesh dependent. You find the commands described in U4.44.01 (AFFE_CHAR_MECA). Quote: '...In any rigour, the application of a nodal loading is physically incorrect and can cause stress concentrations. It is preferable to use loadings distributed.' That is what FORCE_ARETE does: it distributes the applied line force along the chosen line and its nodes.

I assume you applied a line force in the other software (100N distributed along the edge) and a FORCE_NODALE here (21 nodes in node group in model--> roughly 20 fold displacement)?

I re-read your post ad you wrote at the beginning: '....Salome Geom is scaled by meters...'. That is not the case: every FE-software is in principal independent of units (don't know the correct technical expression). It is the user who defines the unit system (N and m, or what I do: N and mm, others are possible as well) by choice of geometric units (basically the unit of your geometric model) and units of force etc.

Cheers,

Mario.

*Last edited by mf (2020-01-17 14:14:03)*

Offline

**Jan Goebel****Member**- From: Mannheim
- Registered: 2016-04-02
- Posts: 52
- Website

Hi Mario,

thank you again for your big help. So we're getting closer and closer to the solution. By changing the BC to FORCE_ARETE I get a displacement of 79 mm. That means results are still to high, but this time it's the factor 100. So I suppose that there's something wrong with the units, or with the scaling, but by checking evrything, I can still not spot out the mistake.

So here's the exact proceeding of what I did to run this simulation:

1.) Importing Geometry as step file into Salome

2.) All dimensions are displayed as m in Salome, hence I scaled the entire geometry by factor 1000

3.) Setting up/ Modification of the comm file (FORCE_ARETE) with 68000 as for youngs modulus and 0.33 as for poisson ration

What else can be wrong ? I also usually choose N and mm as a unit

Thank you and have a nice weekend,

Jan

Offline

**sameer21101970****Member**- Registered: 2019-09-06
- Posts: 17

try to view .rmed file in gmsh.

open in gmsh.

gmsh readings are same as you are getting in paraview then their is problem.

paraview sometime show wrong reading...you have to adjust the scaling.

Offline