## You are here

# Output of ABAQUS for contact of a rigid surface with a poroelastic layer

Hello, I am modeling the spherical indentation of a poroelastic layer. I am modeling the indenter as a rigid analytical surface. As you know, the total pressure in a porous medium at each point is the sum of the elastic stresses from the matrix, and the pore pressure caused by fluid pressurization. Abaqus provides both the pore pressure and of course the rest of the stress quantities.

As I'm analyzing an indentation problem, my final result needs to be a force quantity (spherical indenter thus non-constant area), or I need to be able to convert the stresses to force by having some knowledge of the area. There are a few outputs that look interesting to me for this purpose, but all correspond with elastic stresses it seems, and not the pore pressure. So if I were only dealing with elastic stresses, I could use CFORCE (CNF2) and sum over nodes for which contact is closed, or alternatively use CFN which is a whole surface output and is the total force due to contact pressure.

These values don't show any stress relaxation however, so it makes me believe that they are not the actual "total" but just the elastic part of the stress tensor. I can't use the pore pressure values and get the force resulting from that part because the problem then becomes converting the pressure to force. I see two output quantities for areas but they don't seem to be useful: CAREA is the "total" area in contact so that won't help because pore pressure varies across the surface. The other is CNAREA which is the "contact nodal area" which is only available for the master surface. This still looks like the most useful to me, but I am not finding any description in the documentation more in-depth than that. Is this the effective area at each node, so that if I multiply the pressure by this and sum over all nodes, I will get what I need (sort of)? I say "sort of" because although the horizontal components cancel out overall (due to symmetry), since I'm looking at each node individually then I will also need to be able to project this onto the z axis for each node.

I'm basically looking for a way to convert the simulation output to force so that it can be compared with the experimental results. Does anyone have an idea/experience with this?

Thanks!

## Hi Roza, Take a

Hi Roza,

Take a reference point in the indenter and then output the total force on the referenc point.

Best,

Yuhang

## Hey Yuhang! Thanks

Hey Yuhang!

Thanks for your response! I tried that before, but that force also does not show any relaxation while it should. That's why I think even the output for the reference point includes only the elastic stresses. Have you done this before in Abaqus? If you're sure that this includes the pore pressure effect too, then I may be making a mistake somewhere. Please let me know what you think :)

Best,

Roza

## Hi Roza, I have done

Hi Roza,

I have done this before without problem.

The force force on the reference point should be overall resistant force from the poroelastic material.

You should do the calculation in two steps.

In the first step, apply the load rapidly, so that a pore pressure field will be built in the sample.

In the second step, apply zero pore pressure on the boundary, so that the solvent will migrate out through the boundary and relax the force.

Another way to do it is: apply no flux in the first step and release the constrain of no flux in the second step.

Any way, the point is a field of pore pressure has to be built up in the frist place. It is due to conservation of solvent.

Hope it helps.

Best,

Yuhang

## Your indentation simulations

Hi Roza,

I agree with Yuhang, I also do similar simulations.

You define a reference point for the rigid surface and run a displacement-driven simulation by applying the indentation depth at the reference point (a two steps simulation: ramp and hold), then you make a plot of reaction force versus time. If your permeability parameters and boundary conditions are correct, you'll get your relaxation response.

If your ramp phase is too long (it depndens on permeability) then during the hold phase you might have a very little relaxation.

Regards

Pasquale

## Thanks, Yuhang and Pasquale!

Thanks, Yuhang and Pasquale!