Convergence analysis and adaptive remeshing

[dw1982]

Hi,

I'm working on a solid contact model involving sharp edges and small surfaces. I am trying to get my results to converge but I can't. I started with a coarse mesh (~8000 tetrahedral quad elements) and refined the mesh by using smaller global seeds in the area of interest while maintaining larger elements on the peripheries of the model far from the area of contact. The maximum stress values increase drastically when I use finer meshes and the values do not seem to converge. Also when I used smaller elements in the contact area the analysis aborts because of excessive distortion of some elements. I finally ended up with ~100,000 elements and the analysis has been running for 36 hours now and I am not even sure if the results will be accurate.

Is there any way to get around this problem? I thought adaptive remeshing might help but it did not reach the goal (5% error max stress) after several iterations.

Any suggestions

 

[johnhors]

You will never achieve "mesh convergence" with sharp edges present. Do these sharp edges really exist?

http://www.Roshaz.com

 

[dw1982]

They do. it's a screw and the threads and tip are sharp. What do you suggest?

 

[dw1982]

Here's a screenshot of my mesh.I know it is very coarse, but when I use finer elements the stresses become unrealistically high. Any suggestions would be greatly appreciated!

 

[xerf]

If I am not wrong, you seem to expect some strong distortion either of the screw edges or of the material of hole.

If this the case, Abaqus/Standard might not be the tool of choice here. Maybe you should give it a try first with Explicit and see what type of deformation you can expect. Do not worry about the stress accuracy at this time.

 

[dw1982]

I am sorry for not explaining this. I am not to concerned about the stresses around the threads since these are stress concentration areas and as I read in other posts the stress will keep increasing as I use finer elements.

What I'm interested in is the max stress in the material around the screw in general (neglecting the stresses around the threads). How can I pick the most adequate element size for this purpose? Can I just create a similar model without the threads and just assume that the results will be similar?

 

[corus]

I'd spend a little time and try and get a mesh with hex elements, preferably linear elements as these are more stable. Your model looks axisymmetric too, though I'm not sure that applies to the loads applied. If it is then use a 2D model. Results wil be much faster. The problem with quad tet elements is that the mid-side nodes can get distorted and so appear as if they have excessive distortion and become 'inside-out'.


corus

 

[dw1982]

Thank you corus for your reply.

I tried to look up similar problems in the forum and I read somewhere you saying that the stress values at the corners may be ignored since they are a result of singularities. Let's say I decide to do this and ignore those values, can I just look at the second stress value in the color contour for comparison purposes? My main purpose is to see how the length of the screw for example affects stresses in the nearby area.

The problem is that I already created and modeled many similar models and working on hex elements or axisymmteric models means I have to start from scracth.

 

[DanStro]

I have worked with people that make scalpels in the past and as sharp as they are there is a standard radius on the cutting edge (R0.002mm is coming to mind but I am not sure) so while the vendor of the screw, or even the drawing for the screw, might say that they are sharp in reality it is not EXACTLY sharp.

So, that being said, you might want to try putting a very small radius on those edges.

From the description of what you are looking for I don't see why a small radius would have a noticeable effect on the results. Even if you are a little off on the actual value.

 

[corus]

The problem definition seems to be a bit vague and looking at the 2nd contour value isn't really going to help when your results are mesh dependent. If you've ran a couple of models with different meshes then pick a location that is close to the area of interest but not affected by your mesh zize and then compare values at that location with your different scenarios.

I'd still spend half an hour looking at the mesh rather than wait 36 hours plus for results you're not even going to be confident about. It's also often useful to run simple 2D models first to get an idea of what is going on before going for the full razzamatazz of 3D models. Even then after running a 3D model you can then say with some confidence that the results from a 2D model are good enough for comparative studies. A little extra time at the beginning can save you a lot more in the end.

corus

 

[dw1982]

Corus,

I followed your advice and worked on a simple 2D model that gave me max stress values that converged easily. Would it be safe to extrapolate from there to the 3D models (i.e use a mesh density that gives similar max stress values as in the 2D model)?

I know for a fact that yielding will not occur under the conditions I am applying, I just want to compare different models.

 

[corus]

It would depend if you really need a 3D model that can be more easily described by results from a 2D model. Do the results from the 2D model compare with the results from the 3D model away from areas of high stress? From what I've seen of your model the geometry looks axisymmetric other than the square block. If that is replaced by a cylinder with radius of half the breadth of the block, are the results generally similar to the 3D model for a coarse mesh? If so, then you can use the 2D axisymmetric geometry and use a fine mesh at the 'sharp' corners, except use a small radius, as others have suggested.

corus

 

[dw1982]

The model is not axisymmetric because the direction of loading is not.
The only two options I can think of now is either to use a coarse 3D mesh with comparable values to the ones obtained in the 2D analysis or to use a fine mesh and ignore the peak stress values. Do you think this would work just for comparison?

I am sorry if I'm repeating myself. I appreciate your help, thanks a lot!

 

[corus]

You can ignore the peak stresses if fatigue is not to be considered. In your case the peak stresses are due to the singularity caused by the geometry, which you can't capture anyway. I'd use a mesh that gave results that gave smooth contours in regions of the model I'd be interested in.

If your job is taking a long time to run and has contact in it, then check the time steps it's taking as these may be very small. Contact controls can make the job more stable and run faster. In addition, the use of quadrilateral elements increases the bandwidth of the problem and hence the run time and memory requirements. If you have contact in the problem then try and use linear hex elements, but more of them. Contact will converge better, and the job will run faster.

corus

 

[dw1982]

Thanks a lot for your helpful comments. I appreciate it.

 

[loki3000]

what is that model, if i may ask? what it'll be used for?