Discussion Forum

Claire,

I can't test the model because I don't have your modules. In solid mechanics you don't need a continuity bc between domains. Comsol takes care of continuity if you finalize the geometry into a union.

Cheers Edgar

Thanks for your response, Edgar. I tried finalizing the geometry using a union, and the displacement solution is continuous, but there is still a pressure discontinuity between the domains. Here's a further simplified version (no creep nodes, so it doesn't need the geomechanics module anymore) that uses form union.

Hi Claire,

Pressure is generally not continuous at the interface between two different materials.

At such an interface with normal direction z, only sigma_zz, sigma_zx and sigma_zy are continous in general, so that doesn't tell you anything about continuity of p=-(sigma_xx+sigma_yy+sigma_zz)/3.

Best,

Jeff

Thanks Jeff. That makes sense, I wasn't thinking closely about that. The sigma_zz, sigma_zx, and sigma_zy components are continuous in the simplified model, so that's good.

The actual problem I'm solving is more complicated however. For the real case, I’m using topography data and importing the mesh. I’ve made an identity pair between the ice and the sediment and set a continuity boundary condition for that pair. In this case, the sigma_zz component is not continuous between the ice and sediment everywhere along the boundary (see attached). The normal direction is not in the z direction everywhere, but it is close near where the stress discontinuities are largest, so I think there is some problem with the solution. Any ideas about that?

The thing is, even when the stress tensor component in the (usually unavailable) analytical solution is continuous, the corresponding FEA stress computed from nodal displacements is not continuous across elements (in the general case). The FEA stress component will become closer and closer to being continuous as you refine the mesh. Plotting stress components with any smoothing disabled is actually an old-school way of assessing if the mesh is fine enough: if the stresses are noticeably discontinous across element boundaries, that can be taken as a sign that your mesh is not fine enough, see e.g. "Finite Element Procedures" by (my grad school advisor! - "Hello!" if you read this) K.J. Bathe.

Best,

Jeff

Ok, that's good to know. I'll focus on refining the mesh then (I've had problems getting a higher resolution mesh that doesn't have too many low quality elements for this geometry, given the high aspect ratio, but that's a whole other topic).