If the stress is singular (I can't open the picture for some reason) then the finer you make the mesh, the higher the maximum stress will be. Singular stress can occur in sharp corners, close to forces or fixtures e.tc. and are not real stress. Convergence runs are necessary to understand if you have enough nodes in the right places. (general rule for high quality mesh is minimum 2 nodes thru thickness)
I guess that the scale for min and max stress changes in your 3 pictures above.
Set these levels to fixed values so you see that the general stress is the same.
(Probe tool should be used to find and compare values)
The third picture with the fine mesh looks strange.
General stress in the upper ring should be similar between runs a general darkblue color, similar as the lower part, is expected.
But once again, I cant scale up the picture so I'm not sure what the scale says.
Try adding small fillets ain areas of high stress concentrations and you should be able to get a converged solution for the stresses. Sharp/ sudden changes in geometry can result in mathematical singularities which can ause the stress levels to shot unrealistically high. Theoretically, at such a location, the stress should go to infinity but due to the "finite" nature of finite element methods, you see results which shoot up with decreasing mesh sizes in those areas.
This is normal. Fine mesh does not result in higher stresses. Coarse mesh results in larger errors on the low side.
Keep refining mesh until stresses stop increasing. Auto refinement is a good way to go (also works to make mesh coarse where fine mesh not needed).
Also, as mentioned, watch for singularities.
Hey guys! Thanks a ton for the reply. I'm just a student, and our school doesn't teach this stuff. I'm so happy that you all are willing to help. I have tried to fillet every darn thing! but it is still giving me ridiculous stress values at fine meshing. Let's say if the thinest part in my model is 0.5 cm, I set my mesh parameter to 0.25 cm to address the two element thing for that thickness. But no luck! I've posted my files here, I'd really appreciate it if anyone could look at them and tell me where am I going wrong. Thanks a ton.
Notes: The struts / beams are all bonded conenctions, and the telescope is fixed at the three points at the bottom of the base plate.
I ran a couple of tests on your file.
See picture below, this is with 1 cm meshing but without the small radius that you added.
I get pretty much the same overall resuls when I try your 3 different settings.
The stress concentration in the corner of the primary mirror mount has not converged.
This stress is probably not real, but due to the bounded contact condition.
In reality I guess that the base plate are assembled with screws and a bolt connection combined with "no penetration" would give different results in this area.
I didn't use beam element for the tube and perhaps you have a problem with the contacts between beem and solid in your setup?
I also lack some holes in the base plate compared to your original pictures.
Mikael, thank you so much!
Yes, in reality we will be using bolts and threads.
I'm running this thing with 2.5mm meshing now...and it takes an hour to mesh and run! I'm using a i7 3920XM and 24Gb of RAM! I can't believe that I need more processing power and a finer mesh. There must be something in the model that is wrong.
Wait...does it matter the order in which you select the bonded surfaces? For example, I bonded the outer surface of every tube, to the inner surfaces of the holes...but I didn't pay attention which one I clicked first. The static analysis must run under 20g of force from top to bottom....I think you are using 1g only right?
What do you mean when you say the stress has not converged?
How should I connect the tubes to the holes?
Is it possible for you to attach the files back so I can track you work?!
I just opened your file, with the simulation settings as you have done them, i suppressed the small corner radius, set the mesh global to 1 cm and ran the file. You have already specified 20g so my picture is from 20g (196,2 m/s^2).
If you download your own file from above and supress the corner radius then you should have the same setup as I had.
I didn't save my work but if necessary I can download it again and redo it and post back the results to you.
Convergence = minimize the errors produced by a too corse mesh in an area with high stress gradient.
You should read a bit in the help files about singularities and convergence.
I suppressed the small radius because they didn't add anyhing to the simulation but additional elements and nodes to calcule.
I also changed my scale from N/m^2 to MPa (N/mm^2)
The results from your first and second picture are similar to my results.
The only thing is that I don't see any stress in the upper plate in your solution and therefore I assumed that you had some problem with the beam joint and the solid. I used solid elements for all parts.
Now I read your answer more carefully, and you mention that you bonded the outer surface of the tubes to the inner of the holes. This is your problem. With Beam element you can't bond a surface from the beam member. Only the joint (brown points in you pictures) or beam. This also explains your 3rd picture and the strange result in the upper ring. Joining beams to solid is a little tricky and the easiest solution for you is to run the tubes as solids.
Michael, thanks alot. Would you be able to tell me how to do the simulations with beams? Meaning if I turn the tubes to beams, and find the joints, should I remove their bonded connections and then run the simulation? Or I must do something else?
I do however get somewhere around 46 Mpa for MAX stress, a bit more than what you got...but as long as it is under the yield.
You should manually bond the beam element to the corresponding surfaces in the solids. See picture below.
When it comes to the results, you still needs to understand if it's a singularity caused by fixture, bondings or sharp inner edges or if it's actual stress where you need to refine mesh to see if the stress converges.