Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Applying pressure via compressible gasket
Hello all,
I would be interested in any views on this analysis. A very simple mesh is attached to illustrate the problem. We have a ceramic disc with a stepped outer face. The two metal rings are brazed on to the ceramic, but I have not included a braze layer here. The pressure constraints on the two rings come from being clamped between two larger ring components, via two deformable copper gaskets which would sit over the knife edges shown in this model, covering the area that the constraints are applied to. In real life the problem is more complicated, as the pressure is generated by a ring of bolts in the outer (not shown) clamping rings. We want to assess the stress within the ceramic. I have made the assumption here that the copper and the braze spread the load from the bolts so an axisymmetric model is a valid first stab.
We don't actually know the force or pressure from the bolts, so I applied a pressure equivalent to a listed value for the yield stress of copper (around 33 MPa).
When I refine the model shown, it shows little tendency to converge (taking the max. von Mises stress as an indicator), with max stress increasing with each refine, although the assymetry between stress in the upper and lower halves improves. When I use quadratic elements (hex & tri), the von Mises stress is higher with even less tendency to converge (example attached), and when I go for quadratic (tris all converted to hex) there are problems with cracks in the mesh that I have not had the patience to fix.
1. Is my approach to loading a reasonable first stab?
2. What is wrong with the mesh that it does not give sufficiently converging solutions on refinement?
3. Are the internal sharp corners where ceramic meets metal ring a problem?
4. Have I constrained rigid body motion correctly?
If I can get a sensible output from this stage, I think I will need to include thermal stresses from the brazing, which I believe will need a radial symmetry model. I currently have no hand calculations on which to judge my results, but to be getting von Mises stress in the ceramic an order of magnitude higher than the applied pressure does not seem right.
I would be interested in any views on this analysis. A very simple mesh is attached to illustrate the problem. We have a ceramic disc with a stepped outer face. The two metal rings are brazed on to the ceramic, but I have not included a braze layer here. The pressure constraints on the two rings come from being clamped between two larger ring components, via two deformable copper gaskets which would sit over the knife edges shown in this model, covering the area that the constraints are applied to. In real life the problem is more complicated, as the pressure is generated by a ring of bolts in the outer (not shown) clamping rings. We want to assess the stress within the ceramic. I have made the assumption here that the copper and the braze spread the load from the bolts so an axisymmetric model is a valid first stab.
We don't actually know the force or pressure from the bolts, so I applied a pressure equivalent to a listed value for the yield stress of copper (around 33 MPa).
When I refine the model shown, it shows little tendency to converge (taking the max. von Mises stress as an indicator), with max stress increasing with each refine, although the assymetry between stress in the upper and lower halves improves. When I use quadratic elements (hex & tri), the von Mises stress is higher with even less tendency to converge (example attached), and when I go for quadratic (tris all converted to hex) there are problems with cracks in the mesh that I have not had the patience to fix.
1. Is my approach to loading a reasonable first stab?
2. What is wrong with the mesh that it does not give sufficiently converging solutions on refinement?
3. Are the internal sharp corners where ceramic meets metal ring a problem?
4. Have I constrained rigid body motion correctly?
If I can get a sensible output from this stage, I think I will need to include thermal stresses from the brazing, which I believe will need a radial symmetry model. I currently have no hand calculations on which to judge my results, but to be getting von Mises stress in the ceramic an order of magnitude higher than the applied pressure does not seem right.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
1. Is my approach to loading a reasonable first stab? I would make separates parts and apply contact (to allow the part to slide), but don't know if works for axisimetric elements, maybe you can model a quarter or less of the geometry.
2. What is wrong with the mesh that it does not give sufficiently converging solutions on refinement? Guess that is due to the sharp angle and the lack of sliding between the two materials, maybe is generating a discontinuity on the model and then stress will not converge.
3. Are the internal sharp corners where ceramic meets metal ring a problem? Maybe, I would add a radius in that area and do mesh refinement only in that place, but again with separated parts and contact wit sliding.
4. Have I constrained rigid body motion correctly? Looks like the Y restriction on one node is being covered/superimpossed/duplicated by the Y restriction on the 10 nodes
Regards
1. It looks OK to me. I would also try a force parallel to the axis (bolt direction?) in case normal pressure causes artificial radial loading which, in real life, might be opposed by friction between the outer rings and the rings in the model.
2. See 3. Also, a possible problem is the curved edges have become faceted with refinement so they could develop irregular stress patterns which might not converge either. You should smooth the curves after each refinement step using Mesh tools -> Fit to curved surface. Alternatively, start with quadratic elements on the coarse mesh and they'll remain as parabolic curves during refinement. It's not exactly circular but with 2 or 3 elements around a quarter-circle, it's probably close enough.
3. Yes. It's effectively a crack tip with zero radius and theoretically infinite stress. This is one of the most challenging issues with FEA. Some ways to handle this type of problem:
If you expect the ceramic to dig a small groove into the copper and not progress any further then you could ignore this stress. The stress any fixed distance from the corner should be converging and would be a more useful thing to check.
You could use the CalculiX solver with plasticity to model the details of that groove and any other plastic deformation.
If the ceramic doesn't really have a sharp corner, then you can use CalculiX with contact between the copper and ceramic so they're allowed to redistribute the stress by changing the contact area as they deform.
4. Yes
I've started looking at Calculix but it'll take me a while to figure.