[yann97]

Hello,

I am trying to model leaks in an internal combustion engine. I started by producing a simplified version of the piston on solidworks, then mesh it. I am starting to test the model on really simple case (the piston isnt moving, there is only a high pressure up and a low pressure down) but i don't manage to get it to work. I use 2 DFBI body for the two piston rings (that should be moving up or down) due to the pressure gradient.
I chose a really fine mesh in order to have a proper flow throught ring gap, but i keep running into the error "Error: AMG solver diverged.
A floating point exception has occurred: floating point exception [Divide by zero]. The specific cause cannot be identified. Please refer to the troubleshooting section of the User's Guide.
Context: star.segregatedflow.SegregatedFlowSolver
Command: Automation.Run"
I got the following warning 1 iteration before the crash : "WARNING: Ap = 0 on multigrid level 1, nRows = 560339, blockSize = 1
AMG coarsening halted."


I can see I have a problem somewhere because after the 4th iteration, temperature sky-rocket without any explanation, starting in the exact center of the mesh.
I would like to have some advice about what could go wrong, if it were possible. I can provide mesh screenshots if needed.

thanks !

[ping]

there can be lots of reasons for this error and the support site gives good ideas. my guess is that you have separated mesh regions not connected that should be to the rest and so check for this using Pre-Processing > Defining the Regions Layout > Region Manipulation > Region Splitting > Splitting Non Contiguous Regions and if this is confirmed then you need to fix it.
i would simplify the model by removing dfbi regions and see that it runs well first and then add them in again.
and you will want to check you mesh quality since this can cause this sort of failure.

[yann97]

Originally Posted by ping

there can be lots of reasons for this error and the support site gives good ideas. my guess is that you have separated mesh regions not connected that should be to the rest and so check for this using Pre-Processing > Defining the Regions Layout > Region Manipulation > Region Splitting > Splitting Non Contiguous Regions and if this is confirmed then you need to fix it.
i would simplify the model by removing dfbi regions and see that it runs well first and then add them in again.
and you will want to check you mesh quality since this can cause this sort of failure.

I already simplified the model by removing the DFBI body and i already check for non contiguous region. The lower cell quality I have is 0.01 and i read in the Help that i shouldn't go under 10^-5, so it should be ok. Here is a screenshot of my mesh for further help or reference.
https://imagizer.imageshack.com/img922/1013/yAdIT0.png
https://imagizer.imageshack.com/img922/1173/e2UzUD.png

[ping]

you have misunderstood the help on cell quality - 1.0 is a perfect cell and you should aim to be a good a possible .1 would be much better.
but this is only one measure of your mesh quality and it is best to run the reports in the mesh menu to get a better feel.
i would be creating a threshold based on the various quality fields and looking at the cells found and improving the mesh in the bad areas.
also you could add the cell quality remediation physics model since this dampens the effect of poor cells in the solver.
I wonder about your mesh for a few reasons - why is the prism layer not using hexas and this causes large cell volume changes between the prism layer and the rest for no reason.
the hexa mesh is too coarse in the ring groove and gap and at the exit to the gap and also you need to change the hexa cell growth rate to be slower