Support simulation

About the development of the FEM module/workbench.

Moderator: bernd

efyx
Posts: 268
Joined: Fri Sep 26, 2014 7:36 pm

Support simulation

Postby efyx » Wed Jan 09, 2019 9:40 am

Hi,
can anyone look to this simulation of support. Some questions below:
1) How simulation should be done to be efficient, because mesh is so heavy that my computer works very slow. Can this be done by simplifying mesh, and improve only on connection points? How to simulate beams like this (rounds have very complicated mesh). Or this should be done different (as a surface with given thickness from hand) - how to do it? Some example solutions welcome.
2) Connection between beams are filled with weld. This should be somehow added to mesh (how to do it corectly?), or I should just ignore that? That's the place where is the most deformated.
3) If this is rightly done, so how to do complicated structures as a simulation, it may be not possible.


https://we.tl/t-oVvjP0V96V <-- link to model because it is big (80mb)
fandaL
Posts: 320
Joined: Thu Jul 24, 2014 8:29 am

Re: Support simulation

Postby fandaL » Thu Jan 10, 2019 10:08 pm

Hi,
It's not so easy to say what modelling approach is the best (3D or 2D or 1D). It depends on the geometry (how hard could be to mesh it and calculate or recreate for 2D from 3D) and how precise results you need. For models like this I would make simplified 2D model (without radii) and make FE analysis with shell elements (for output use "Beam Shell Result Output 3D = true" in the CalcluiliXccxTools) and prescribed thicknesses - see attachment. 3D model is possible and for "good" geometry it can be faster to prepare, but stuff like small fillets or gaps which are not welded could make problems as well as small wall thickness.
results_with_shell_elements.png
results_with_shell_elements.png (66.89 KiB) Viewed 272 times
In general you can use local mesh refinement (the tool in FC: FEM mesh region) in the areas of interest and rough mesh where you don't care much. Especially for large models it is good to think about the symmetry and make e.g. only the half of the model with proper boundary conditions on the mirror plane.
uchwyt2.FCStd
(57.13 KiB) Downloaded 8 times
Attachment file has cleaned mesh (right click on the mesh object -> Clean FEM mesh) - you can simply recreate it and recalculate.

If the gravity load is small in compare to the external loads, self weight is often neglected. I was not sure if you prescribed it in the correct direction - minus Z?

There was also one nice example of the tube connection on the forum which I could not find.
User avatar
HarryvL
Posts: 823
Joined: Sat Jan 06, 2018 7:38 pm

Re: Support simulation

Postby HarryvL » Fri Jan 11, 2019 8:12 pm

Hi @efyx, a few comments in addition to what @fandaL offers:

1) I like your mesh !
2) If you delete the result objects and meshes and clear the input mesh then you end up with a 43kB file rather than a 80MB file.
3) Did you lose your sketches somewhere in the process? It would be good to know the dimensions of the tubes and support plates.
4) In the good old days you would design this type of detail with a pencil and piece of paper. The bending moments, shear forces and torque follow from simple static equilibrium. The deformations at the tip would come from a cantilever solution with a rotational spring at the support. This spring stiffness would probably take a little effort to figure out, but again comes from a standard torsional solution.
5) The torsion shaft between the two supports does nothing for symmetric loading (so I would even go further than @fandaL and leave it out). For asymmetric loading it also contributes little, because the load from both sides is mainly taken out at the supports.
6) So, for global deformations, shear forces, bending moments, torque and support reactions I would definitely not use more than 1D elements (in fact it is quicker by hand).
7) For local stresses at the various connections you could use either 2D or 3D elements (for welds you would be stuck with 3D), but need too think ahead of what you would allow in terms of stresses. See the discussions here https://forum.freecadweb.org/viewtopic. ... 31#p220381 and here https://forum.freecadweb.org/viewtopic. ... 31#p220591 and here https://forum.freecadweb.org/viewtopic. ... 10#p217518
8) Finally, this is how I modelled tube connections in 2D: https://forum.freecadweb.org/viewtopic.php?f=24&t=26921 and in 3D: https://forum.freecadweb.org/viewtopic.php?f=24&t=27431

Hope this helps.

Harry
User avatar
HarryvL
Posts: 823
Joined: Sat Jan 06, 2018 7:38 pm

Re: Support simulation

Postby HarryvL » Fri Jan 11, 2019 8:30 pm

HarryvL wrote:
Fri Jan 11, 2019 8:12 pm
5) The torsion shaft between the two supports does nothing for symmetric loading (so I would even go further than @fandaL and leave it out). For asymmetric loading it also contributes little, because the load from both sides is mainly taken out at the supports.
Urrrrrrr ... this is not true for bending of the support plate out of its plane, i.e. twisting around the y or z axes:


Model.jpg
Model.jpg (48.5 KiB) Viewed 231 times
efyx
Posts: 268
Joined: Fri Sep 26, 2014 7:36 pm

Re: Support simulation

Postby efyx » Tue Jan 15, 2019 11:17 am

fandaL wrote:
Thu Jan 10, 2019 10:08 pm
This is fantastic, this example show exactly how to use 2d mesh. Thanks. How to determine min and max size of mesh? You set it for 20 and 20.
HarryvL wrote:
Fri Jan 11, 2019 8:12 pm
3) Did you lose your sketches somewhere in the process? It would be good to know the dimensions of the tubes and support plates.
Actually this is step file so sketches are not available. But especially I did another issue. Please see below. I'll study your links but few are not working. Thanks.
HarryvL wrote:
Fri Jan 11, 2019 8:12 pm
4) In the good old days you would design this type of detail with a pencil and piece of paper.
Yeah, but this is faster, easier and less chance to do something wrong ;)

This is another issue. Let's imagine lifting arm. It is rotating around first hole (near the edge) (not supported). Actuator is pushing the second hole (ear) on angle 45 deg. The load is putted on the end. How to fix rotating point to simulate what will happen to the beam in the reaction of force, while whole arm is rotating.
lifting_arm.FCStd
(17.95 KiB) Downloaded 5 times
fandaL
Posts: 320
Joined: Thu Jul 24, 2014 8:29 am

Re: Support simulation

Postby fandaL » Thu Jan 17, 2019 10:19 pm

efyx wrote:
Tue Jan 15, 2019 11:17 am
...
How to determine min and max size of mesh? You set it for 20 and 20.
I just chose the size which "looked good" to me for the beginning. It is not bad practice to run the new model with finer and finer mesh (which is easy in FreeCAD due to work on geometry and not directly on the mesh) and if there would not be a singularity, you will see mesh convergency - from some size the results will not change significantly. Different behaviour is if there is some singularity - stress concentration in the sharp corner or under the point load - in that case refinement of the mesh would lead to extreme stresses with linear static analysis which does not make practical sense. This was discussed somewhere on the FC forum or there are for sure nice articles and blogs explaining it, e.g. by quick search:
https://andreweib.wordpress.com/2010/12 ... ularities/
http://www.acin.net/2015/06/02/stress-s ... nvergence/