analysing details (a thread in this case)

DRQ

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

Sergio

I would sacrify a little of accuracy using half, or cuarter part if the loading is simmetric, best would be an axissimmetric model. Looks like your elements has not the best shape, I have a feeling that bad shape element can increase the time to solve. My votes are for an axisimetric model meshed with mainly second order cuad, there you could use a very fine mesh.

https://www.dropbox.com/s/47tarv4r5nqv1d5/Chapter03.pdf?dl=0

DRQ

Hi Sergio,
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!

DRQ

I did make some progress over the weekend since my original post. I got a much better looking mesh by using gmsh through Mecway. I'd previously tried using gmsh completely stand-alone, and then import the mesh in Mecway but I'd made mistakes in the settings which Mecway has avoided.
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.

Sergio

Sometimes for a huge mesh like I imagine that is your case, CCX PARDISO shows me as a succefull run, but not results are stored, this is due to the fact that you don't have enough RAM memory. You could try using the internal Mecway solver, that will be slower to solve, but can manage models that doesn´t fit in RAM.

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.

Victor

I'm not aware of any cases where the internal solver gets stuck forever. It can take a long time at some steps but it should eventually either succeed or fail with an error message if you leave it long enough, which could be up to a day.

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.

JohnM

The spiral sweep for threads works but you will find you need to leave a pin hole down the center of the bolt. Another option is to leave a larger cylindrical dead volume and fill this void with tet/pyramid elements. Also, you will find the beginning/end of thread root will need some manual work or tet fill. Do-able, but not easy!

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.

DRQ

I've not had access to the forum for a couple of days so am catching up. Thank you for your comments.
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:

1. with an undercut / thread relief so that the cutting tool has somewhere to go
   
2. run the thread out, as if cutting tool is pulled away from the bar stock so the cut gets shallower
   
3. stop the thread, as if the thread is being ground into the stock, with the feed and the workpiece rotation stopped but allow the grinding wheel to still rotate
   

I've probably explained that very badly.

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.

Sergio

If your models will differ only in the transition area, you could do a first analysis with a medium size mesh, and then do a submodeling analysis with a finer mesh only in that area, the good news is that you can use the same first main analysis for the three versions.

For making the axisimetric analysis, you could import a surface model directly, not curves as DXF.

DRQ

Sergio, thanks for the tip about surfaces. I don't use very often, probably never! so I wouldn't have thought of it.