(average)nodal stress skewed?

[321GO]

On my assembly the location with the highest stress occurs at the mating between two components. When comparing nodal vs element value's there is a large difference.

Is this normal behavior? To my understanding yes, because of the inherent differences on both "sides" of the mated components, which results in non egual element stresses(on shared nodes).

Do the averaged nodal value's become skewed and is it best to use element stresses in such transition locations?

Thanks in advance...

 

[EngAddict]

No, it is best to use the nodal stress. Element averages the stress across all the nodes, so if you have a large difference in the stress then your model is not very accurate. You will need to refine your mesh further. You can also use the error plot for this.

 

[kellnerp]

It is incorrect to say element stress averages the stress across its nodes. That is not how FEA elements work.

An element enforces displacement continuity between elements, not strain continuity. Element stresses are calculated at the gauss points which are not the same as nodes. For each element the stress at the gauss point is more accurate FOR THAT ELEMENT. Because Gauss points are internal they reflect a state of stress in the element away from the nodes and based only on the displacements at the nodes. In areas of high stress gradients the pattern of displacements between to adjacent connected elements can result in greatly varying stress results at both the gauss points and the stresses are extrapolated to the nodes. So if you look at the nodal stress results JUST for a particular element and then look at the nodal stress results for the same node as calculated by an adjacent element you can get widely differing nodal stresses. The software uses a scheme to average nodal stresses taking the contributions from adjacent element nodal stresses.

Depending on how your two parts are mated and in fact on what materials they are made of, averaging nodal stress at an assembly interface is not a good idea. For example, if one part is aluminum and the other beryllium then for the same strain (calculated from nodal displacements) the stress in the aluminum will be 1/3 of that in the berylium assuming a bonded connection between the two.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[321GO]

kellnerp,

in my understanding element value's are ok to use, as long as the results are converged.

If, results will continue to differ even after convergence, one can assume that nodal value's cannot be used(at this specific location) and element value's should be used.

Since this is the case, it is best to use the element value's in stead.

Do you agree?


Thx in advance again!


p.s. no matter how fine i mesh(at the intersection of the mated surfaces) nodal and element value's simply will not correlate. When making a error plot, there is also an error right at this location.

 

[EngAddict]

ok, it is not 100% accurate but element stresses are discontinuous compared to continuous node stresses. Hence node stress are considered to be the more accurate 'exact' stress.

You might find there will always be some error and it is not an absolute sign of convergence anyway. You should check convergence manually to make sure the stress is accurate.

 

[kellnerp]

If, results will continue to differ even after convergence, one can assume that nodal value's cannot be used(at this specific location) and element value's should be used.

For the reasons I have given, the nodal stresses will almost always be different from the element stress. So by the logic you are using nodal stresses should never be used.

In CosmosWorks, the element stress is itself an average. You will have to run your model in Cosmos/M to get the actual elements stresses at the gauss points.

You also need to state what problem you are trying to solve in doing what you are doing. If it is fatigue you will most likely want nodal stresses.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[321GO]

Hello kellnerp / EngAddict,

yes i agree, but in my understanding the difference would normally be relatively small(after convergence).
In this particular case i do find the difference to be large.

I attached the convergence for both cases.

Or is this normal behaviour?


Thx in advance.

 

[corus]

I'm not sure what the probloem is as it seems obvious to me that nodal and element stresses will be different as they occupy different positions.

In your graph, I would query the last result as it seems not to fit the general trend of the previous results. In general it appears that as you refine the mesh, the stress increases. This indicates some sharp discontinuity for which stresses will tend towards infinity. If it's not fatigue damage you're looking for then I'd class the stress at that position as being a feature of the model and not relevant for structural integrity.

ex-corus (semi-detached)

 

[321GO]

Hi corus,

thank you, and yes this seems to "become" a singularity issue.
The restraint on the inner hub part seems to be causing this(zero movement in axial direction restraint).

Fines Mesh -> Higer stresses, i attached the situation more precise. The fringe plot confirms this also(jagged).

I'm not sure how to solve this though, since the stresses are relevant in this area.

Thanks to all again for your suggestions/advice!

 

[EngAddict]

Use Iso Clip and see what your actual highest stress is.

Do you have the pressure vessel module? If not you can manually linearize the stress to isolate the peak stresses.

Are you interested in fatigue at all?

 

[321GO]

Hi EngAddict,

thanks for your response,

No, fatigue is not an issue, but i do need some idea of the stress at this location since it obviously present.

I'm trying different approaches and it seem to make a lot of difference if i model the innerhub(node to surface condition) or to replace completely with a virtual wall condition.

The latter provides much better results, which puzzles me a lot since they should behave equal, right?

So, it seems that results are better if i remove the innerhub and apply a virtual wall, but why?

Has this to do with the interaction of the two separate meshes?

Thanks again in advance!

 

[kellnerp]

Have you run a check on your mesh? Unless you have modeled a crack there, a small hot spot in that kind of geometry and loading is a tipoff that something is wrong with the model.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[321GO]

Yes, i did, mesh should be fine, aspect ratio < 4.

Although i had to use the alternative mesher to get it this low for some reason.

Could it be that the alternative mesh is causing difficulties on the node to surface condition, although i don't see why it should.

 

[321GO]

Hi all,

pls take a look at the attachment.

kellnerp, you where probably right that the mesh was/is the problem.

Although i now probably have some discretization error, the results seem much more viable.

Thought's more than welcome!

 

[corus]

The problem of high stresses occurs because you have applied a rigid restraint along a face. This has the same effect as if you had a sharp discontinuity there. It's generally wiser not to apply a fixed restraint adjacent to an area where you're interested in the stresses, for that reason. If you have contact between two bodies to apply the restraint then that might 'soften' the restraint there and give you more reasonable stresses. The jagged contours are a feature of tet elements unfortunately and there's not much you can do about them other than have a very fine mesh, or use a different FE package with brick elements.

ex-corus (semi-detached)

 

[321GO]

Yes, i have placed the new restraints not on the actual inner hub but on an adjacent part, away from the location. This indeed "softens" the transition somewhat.

Although i'm quite supprised that the coarser mesh gives better results, Cosmos simply will not mesh nicely when using finer elements.

When using the finer mesh, the stress is very jagged and locally very high, which cannot be correct. But i'm not quite sure what is causing this problem, the distortion in the mesh or the overly stiff restraint. To my understanding an overly stiff restraint would induce high stress(singularity), but uniformly distributed along an edge, which is not the case here since results are jagged.

When using the somewhat bulky mesh, results seem fine except for the possible discretization error.

 

[kellnerp]

One thing in SW is to run tools/check for slivers and small edges. That kind of thing will give a mesher fits.

Second, you can use split face to localize mesh refinement. You can also use multibodies to control meshing too. In fact you could had the spacers between the rotor faces real coarse and bond them.

Third, the mesh in the area in question still looks funky, but you never can tell with tets. This part would be amenable to hex meshing but cosmos doesn't have this functionality.

When you use mesh refinement, tell it to use more than 3 layers to transition. That can help with element shape. Use a smaller factor too.


Can you post a section view cutting with a plane containing the axis of the rotor? It is hard to tell what kind, if any fillet is in the hot zone.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[321GO]

kellnerp,
thanks for the tips, and yes i have splitted the fillet for mesh control already.

The hot spot is indeed a filled and it is the one connecting the hub to the collar portion(the zoomed in fillet in the last attachment).

Also, surface is checked for short edge < 0.001mm and no problems here also.

For the finer mesh run i already used an ratio of 1.1, even then fine mesh is more distorted than the coarse one...

I also checked to make sure the radii are tangent to the adjecent surface in the SW model, they are all mated.

I will try the multi body though.


p.s. the finer mesh creates larger Aspect Ratio's then the coarse mesh(mayby this was not clear from the attachment).

 

[321GO]

kellnerp,

a cross section of the area is attached.

Will try;
1) remove friction on inner contact surface(this was mu=1), maybe this will make the restaint more "soft" and realistic

2) replace restraint from inner to outher flange surface

 

[321GO]

Hi all,

what i've got is not a solution but in my opinion the best i can do here, pls let me know what you guys think.


Again, thx in advance.

p.s. the main problem was the stiffness of the restraint, not so much the mesh distortion