I’ve set the friction to 0.3 and the gap conductance to 100 (as in the Calculix documentation).
I’ve also changed the mesh to second order and get (in PrePoMax): C3D10.
According to the Calculix documentation for thermo-mechanical simulation I should have a C3D10T element type, so I understand that in the INP file I’ve to change the element types accordingly.
I’ve conducted the calculation without changing the element types from C3D10 to C3D10T and effect is like depicted on the image – actually nothing happens:
I do thank you Sir for the willingness to help me. Unfortunately as a user I’m not allowed to upload any code via Calculix or PrePoMax discourse group so please find below the link to the PMX File from my recent simulation.
If you want to allow the rotation of the disc, you have to apply the boundary condition with unconstrained UR2 via rigid body constraint. Applying it directly won’t work since solid elements don’t have rotational degrees of freedom.
Enable Nlgeom and prescribe the rotation as a boundary condition instead of a centrifugal load.
Change the incrementation to automatic.
Add mechanical quantities to output requests so that you can see what happens in the model.
You may have to replace the pressure acting on the pad with displacement BC pushing it towards the disc (at least in the first step, then you can remove this BC and add pressure in the second step). Otherwise, there will be rigid body motion leading to non-convergence.
You should add *GAP HEAT GENERATION using the keyword editor if you want to model frictional heat generation.
I do thank you very much Sir for checking the model and all the mentioned above suggestions / remarks regarding its content.
I will carefully study it and try to understand and implement, but please allow me to ask 2 questions already now, as I know that I will not be able to find an answer myself, i.e.:
The issue with rotating degree of freedom for solids is already one which I do not understand fully – is it related only to PrePoMax / Calculix solver, because I think that in other FEM software solid elements in 3D have normally 6 DOF (you mentioned about the missing rotating DOF in one of your lectures but I could not find the explanation for that).
The item No. 5 is a little unclear for me: now I have one single step where both loads:
pressure on the PAD (pressure value + allowed movement in the Y direction)
rotation (tabular rad/s figures + rotation around Y axis)
are active (similar to the Abaqus tutorial from Abaqus Acumen).
Should I divide those 1 step in 2 separate steps i.e.
first step only for pressure (with perturbation keyword to act on further steps) ?
No, it applies to FEA in general but some programs (usually less professional ones like CAD-embedded FEA modules) seem to be applying moments and rotations directly to solids while internally they use tricks like rigid constraints or cylindrical coordinate systems. Abaqus also requires users to apply moments/rotations to solids via rigid body or coupling constraints. Solid elements with rotational DOFs are very rare, I’ve only heard about a single program featuring them.
To avoid issues with initial rigid body motions, it might be best to do it this way:
step 1 - rotation of the disc and prescribed displacement pushing the pad towards it
step 2 - further rotation of the disc and pressure applied to the pad which should already be in contact with the disc after step 1
I do thank you Sir for both answers - the issue with reduced DOF for solids in FEM is actually new for me.
Will have to learn more about this - thank you very much for the hint.
Will now try to implement in the model all the received suggestions - thank you very much for all of them.
I’ve tried to possibly fulfill all your suggestions + I’ve changed the element type from C3D10 to C3D10T.
I’ve done this in vim and also I’m running the calculation on a separate machine and then just transfer the FRD file back.
The calculation stops automatically with errors.
I’ve noticed that know the Disk is rotating around the Z axis what is pretty strange for me, and I will check it once more.
Please allow me one question as I’m not sure if I do understand it correctly.
The STEP block is one complete simulation, so in my case the PAD pressure and the disc rotation should be included in 1 common step.
The PERTURBATION keyword (and by that many STEPS) should be only use in cases where pre-loading is needed e.g. modal calculations - so not in my case.
I’ve downloaded my FRD file and also the INP file on the google drive like yesterday – maybe you Sir could once more have alook at it and give me some further recommendations.
A step is just a phase of the analysis. A single simulation can consist of multiple steps that are either independent (linear perturbation steps) or dependent (general steps) on each other. So you can have one load in the first step, then deactivate or keep it and add a different load in the second step. That’s what I suggested to avoid rigid body motions caused by the fact that the pad is unconstrained in the direction towards the disc (only pressure is applied but no boundary condition in that direction). And yes, the PERTURBATION parameter is not relevant in this case.
This input file has some unusual syntax (no keywords). Can you share the one exported from PrePoMax or (better) the new .pmx file ?
