Hi,
I guess the title might have put a few people off, I know threads aren't often modelled in FEA but in this case I'm trying to decide between different designs of the area between fully threaded and plain diameter. I'm not trying to model the threaded joint itself.
This is a design in progress, so there's no actual hardware at the moment.
The thread itself is M8 x 1.25 and needs to become a plain diameter of just under Ø8mm diameter.
I'm having difficulty analysing this with the level of detail that I think it needs. Does anyone have any suggestions? I've just managed to get a solution using a mesh generated in gmsh and imported into Mecway, then used the CCX solver, but I think that's overlooked a lot of problems in the mesh.
Does anyone have any tips for analysis of fine details? Is one mesher better than the others at this sort of things?
Any help will be appreciated.
Regards,
DRQ
Comments
https://www.dropbox.com/s/47tarv4r5nqv1d5/Chapter03.pdf?dl=0
Thanks for taking a look at this. I'm deliberately not using an axisymmetric model because I think that making that approximation would lose the details that I'm concerned with, i.e. in the thread. I'm sure you can imagine that an axisymmetric version would treat the thread as being a all the way around, the diameter would be increasing and decreasing and I don't know that that would give me any insight into how the thread ends.
I would normally use axisymmetric, and have modelled the rest of this part this way but for this detail I don't think it will help. I could be wrong though!
But I'm having issues with solvers:
Mecway internal solver either gets stuck at "allocating matrix" or, with a coarser mesh, goes through to solving matrix and was there for about 20 minutes before I had to pack up (I can try leaving it for longer, if that seems sensible)
CCX SPOOLES gives "ERROR in u_realloc: error allocating memory" - I wonder if this is related to the "a correction to SPOOLES.2.2 for large input decks" problem?
CCX PARDISO appears to work with "Job finished" but I don't see any results, do they have to be loaded separately? I checked for an .inp file but could find one.
You could try to tune your mesh to have bigger elements at the core and smaller at the threads, I have seen even some people that has made separated meshes for the core and threads, and glued by TIE. Meshing separately would allow you to use hexa elements and decrease a lot the element count.
Now, seriously, If I have to weigh all the headaches and time to make solve accurately a solid mesh...I would choose again the axissimetric model, even you could do several ones to take in count different sections of the thread as the case for the end.
Just a thought - have you considered building the mesh manually in Mecway using Mesh tools -> Sweep? That can make spiral shaped extrusions with a changing radius if you first define the path with line elements. Perhaps also with a separate cylindrical core like Sergio suggested. An advantage is you can get well shaped hex elements from it.
I'm with Sergio on this- I may not understand your particular need but I have modelled many a bolt thread in my career - axisymmetric or a swept axisymmetric mesh is very effective at assessing thread stress, and you will see very clearly the peak stresses in the root fade over 3-5 threads, same as the way they fail.
I ran the internal solver again and left it. After several hours it did solve the model that PARDISO solved (but didn't show results for). I then tried the model with the finer mesh that PARDISO couldn't solve and the internal solver also gave a memory error, "Error: P-9 Insufficient memory for matrix solver" which at least gives a better explanation.
I can look at different ways of building the mesh but JohnM has highlighted the particular concern I have.
I'm looking at this not to investigate at the stress in the thread but more in the area it transitions from the thread to the parallel cylindrical portion, so the "the beginning/end of thread root" in particular. I've got three main options to compare:
It's version 3 that's got me really focussed on the full 3D model, since I can imagine that the stress concentration where the thread stops could be high, and that's just in one circumferential location.
I do plan to try with different mesh through the body, once I figure out how.
But... I did try to do an axisymmetric model. But the DXF didn't import fully, the flanks and root of the thread are splines in the DXF and these are missing when I import it to Mecway. Am I doing something wrong there? I would like to try this if only to prove to myself that it's a good way to do it.
In the meantime I will try a sector of part as a 3D model.
For making the axisimetric analysis, you could import a surface model directly, not curves as DXF.