[-nan]

Hello,

I have been working on a mixing reactive flow problem. Currently I get ~5 cycles and get the error "WARNING ... extrapolating on the temperature calculation" and then seg fault.

But if I reduce the base grid size by a lot it goes away. Is there some convergence criteria that is not being hit with the small grid? I am using the default parameters for the energy eqn.

Thanks

[Yaju]

Some part of the geometry might not be getting resolved adequately with your coarse mesh setting. This can lead to cell pairing in your simulation and you can get the temperature extrapolation error. When you are refining your grid, these problematic cell pairs might have been removed.

Try to see in you geometry if there are some narrow areas which require extra refinement.

[-nan]

Thanks,
Sorry, I wasn't very clear. The problem goes away if I coarsen the grid. With my refined grid I get the temp. extrapolation error.

[Yaju]

OK. Can you provide brief details on what happens in the simulation (geometry details, physical models being used etc.)? Also, can you please share the logfile (screen output when you run the code) of your case with screen_print_level =2 in inputs.in.

[-nan]

Yes, so my geometry is a box(1mmx10mmx.1mm), the top and bottom are 2D BC, the sides full slip, one outlet, and the inlet is broken up into three sections, where certain species come in through one middle section@some vel, temp. and other species enter through the other two sections, which are on either side of that middle section. I have a dirichlet pressure BC at the exit and neumann BCs elsewhere at the exit and side walls.

My only physical models are Combustion(SAGE with a 37 species 127 rxn mechanism-Thermo and transport .dat provided) and turbulence with default RANS. I have time-based fixed embedding-scale 4 at the inlets and AMR for temp. I usually have AMR for a few species but I had turned it off while debugging.

Attached is my logfile with screen_print_level 2, I had to split it in two and zip it.

Thanks for any help

[Blanco]

Hi,
I'll give my 2 cents, if you look at the log file you can notice that time-step is set to minimum already in iteration 1, because of diffusion constraints. Indeed, ustar and turbulence did not converge, the maximum number of iteration was exceeded. In each following iteration the time-step is still at its minimum and the same problem can be noticed for turbulence and ustar, until everything blow-up at iteration 4. I think you have to try to better initialize your domain, and maybe set a lower minimum time-step that could be used as first time-step as well.

Regards

[-nan]

Thanks,
Yes, I have been looking into better initializing my domain to help with convergence. I am planning to take a coarse simulation that reaches steady-state in my area of interest and mapping that.

[-nan]

Thanks both for your help/suggestions.

I have mapped a previous temp, vel, and species field for better initialization and decreased the time step.

These worked to develop the flame temperatures I was expecting and ustar and turbulence solvers were converging. Still some issues, but the temp. extrap error seems to have been mostly time-step related.