Elmer Discussion Forum

Could somebody help with advise - what need foresee for 3D simulation for Maxwell material under time dependent Border force action?

The 3D layered cube continue it's deformation in direction previously given by Body force after stopping action. For condition elastic cube (without Maxwell material) deformations stop immediately after termination force action. For 2D rectangle there are no problem with non-stop deformation during time dependent viscoelastic simulation.

Thanks in advance!

Hi,

Looking at your mesh, and assuming the unv file was created with gmsh, you probably need to add 'coherence' to your gmsh geo file. Search the elmer forum for posts containing 'coherence' for examples of using that command.

In particular, notice how the nodes between the second and third layers don't line up.

Rich.

If you are using salome it is the merge node command.

In transient accelerations and velocities are include, so if you put a structure under load and it starts moving, then after taking the load of the nodal points have momentum and would still move, unless another force, such as gravity, slows them down, or there is damping.

Also linear tets don't perform well in stresssolver need p2 elements or quadratic (10 noded tets)

Rich_B wrote: ↑23 Sep 2021, 16:15 Hi,

Looking at your mesh, and assuming the unv file was created with gmsh, you probably need to add 'coherence' to your gmsh geo file. Search the elmer forum for posts containing 'coherence' for examples of using that command.

In particular, notice how the nodes between the second and third layers don't line up.

Rich.

Rich,

thank you for instructions! That's a point, after merging nodes, simulation going in proper way, the deformations stopped with load removing after finish given loading time.

Especially for me was usefull your "merge" command instruction for ElmerGrid and application it in ElmerGui at some of advised forum posts.

Also, may be you can advice some Elmer command how to divide a single body in Elmer for containing several bodies which come in unv file after meshing compound of several solids in salome? The problem is - if make tetrahedron mesh separately for each body and after compound them, it is difficult use "merge nodes" command, because there are different mesh sizes for each single solid. To decrease mesh size not a reason due to very large computation time require.

Thank you in advance.

kevinarden wrote: ↑24 Sep 2021, 17:03 Also linear tets don't perform well in stresssolver need p2 elements or quadratic (10 noded tets)

Kevin,

thank your for advice.

Yes, i used salome, and now start pay special attention to "merge node" command.

So i see, need tetrahedron mesh and sorry for my not skilled question, what is it mean p2 elements?

I've understood, that for time-dependant process "transient" most convenient, look's like that's wrong understanding, could you advise what's better instead?

Thanks in advance.

If you do not want to merge nodes at boundaries you can use mortar conditions to connect the boundaries.

See Chapter 9 of solver manual

https://www.nic.funet.fi/pub/sci/physic ... Manual.pdf

Another approach in Salome is to model the whole domain as one block then partition the block into the different bodies. Avoids having to do a compound mesh and each partition of volume elements can be put into a different group. Each group becomes a body in Elmer. Maintains shared nodes at the boundaries.

P2 elements are higher order elements that creates more degrees of freedom internally for higher accuracy, it does increase computation time.

See Appendix E of the solver manual
https://www.nic.funet.fi/pub/sci/physic ... Manual.pdf

They can be turned on in the simulation section of the sif file with
Element = "P:2"

The other option is the 10 noded tetahedron, if you use ElmerGrid to translate mesh you can use the -increase flag and it will convert linear elements to quadratic elements

Salome also has the Modification Convert to/from quadratic to change the linear tets to quadratic tets prior to exporting the universal file.

Hello,

For information about Salome and multiple bodies, take a look at this youtube video from 2015:

https://www.youtube.com/watch?v=xfMLtywHSr4

Rich.

Hi

Mortar method may indeed be used to ensure continuity between nonconforming meshes. There is a rather heavy price that you pay in that the problem becomes a constrained one which means trouble for the linear solvers. At best scenario you need a little more iterations but often the solution time grows considerably. So if possible, try to make a conforming mesh during the mesh generation process. Sometimes it is of course not possible. One such case is rotating machines but luckily earth is rotating only around a fictional axis.

-Peter