[ThunderstruckGER]

Hey everone,

I managed to get my chtMultiRegionFoam case "runnable" since I last posted on this forum - or at least I thought so. I could use your help with analyzing the case and the mistakes I made.

Please keep in mind that I'm trying to teach myself OpenFoam for a project, so my mistakes are probably quite stupid =)

I have attached the latest case file to my post and you can read about what I'm trying to do in this post.

The current problem:

The solver is able to load every input file, yet it crashes after calculating the enthalpy of the first solid region with an "nan" error (.txt attached in case file). So far, I was not able to find an answer to this problem on this forum.

What I tried so far was reducing deltaT in the controlDict, which did not work. Then I tested the case with radiation turned off and played around with maxCo and relaxation factors for h and hFinal as well. But maybe I haven't set those values the right way.

Could the problem originate from wrong boundary conditions? I'm sure there are mistakes in my boundary conditions, but I can't even progress towards a "complete" simulation and trouble-shoot the results. Also, for the current problem I don't have an error message to work with... =/

I would be glad for any hints. Thanks for your help in advance!


0.zip

constant.zip

system.zip

log_crash_nan.txt

[Bloerb]

I am unable to start your case. I am perplexed that you can though

A few hints. Drop the changeDictionary stuff. Make sure every boundary has a boundary condition. For example: Open your case in paraview (paraFoam -builtin). Look at the ACC region.
It has 4 boundaries

inlet
systemgrenzenTopBottom
systemgrenzenFrontBack
ACC_to_nitrogen

assign your best bet to those. Do not use wildcards anywhere. So no "*". And upload your boundary conditions again. This makes it easier to check.


E.g

You specify a flow rate at the inlet. ACC_to_nitrogen is the outlet hence zeroGradient for U. Everything else is a wall. You do however not set a pressure at the outlet ACC_to_nitrogen. zeroGradient on all patches for p_rgh and fixedValue for temperature at all walls. This can't work. Do i have the correct files?

[ThunderstruckGER]

Hey Bloerb, thanks for your reply!

Originally Posted by Bloerb

I am unable to start your case. I am perplexed that you can though

Damn, that's my bad! m(

Forgot to mention I deleted the large polyMesh folders in constant so the file size stays within the upload size limit... I'm sorry about that! So either you can execute blockMesh and then splitMeshRegions -cellZones -overwrite, or I could send you a Dropbox Link/E-Mail instead.

Originally Posted by Bloerb

A few hints. Drop the changeDictionary stuff. Make sure every boundary has a boundary condition. For example: Open your case in paraview (paraFoam -builtin). Look at the ACC region.
It has 4 boundaries

assign your best bet to those. Do not use wildcards anywhere. So no "*". And upload your boundary conditions again. This makes it easier to check.

Yeah, you are right. Seems reasonable and should keep everything more orderly. Concerning the changeDictionaryDicts: I did only use them to generate the 0-files at the beginning of my work.

Originally Posted by Bloerb

You specify a flow rate at the inlet. ACC_to_nitrogen is the outlet hence zeroGradient for U. Everything else is a wall.

So, does every connected fluid region get its own inlets and outlets for U and p? If that's the case, unfortunately I could not come to that conlusion by the tutorials I based my work on =/

I looked into the boundary files in the polyMesh folders I mentioned before. Inlet & oulet are defined as patch, every "system boundary" is a wall and the internal boundaries between the regions are set as mappedWall. Is "mappedWall" the way it should be? blockMesh didn't let me define internal faces when I build my geometry in blockMeshDict.

Originally Posted by Bloerb

You do however not set a pressure at the outlet ACC_to_nitrogen.

The outlet of my whole system is the bottom annulus of the nitrogen region. The pressure at the inlet and at ACC_to_nitrogen is unknown and I want to model the pressure drop across the ACC textile with Darcy-Forchheimer (see fvOptions in ACC). To achieve this, I wanted to set a velocity at the ACC inlet and an ambient pressure at the nitrogen outlet (the bottom annulus) and let the solver calculate all pressures in ACC and nitrogen. I wanted to use calculated as pressure bc for every boundary except the outlet. Have I been on the wrong track?

Apart from that I accidentally have set the bc of p at the outlet in the nitrogen region as calculated. I changed that to fixedValue now. (Nothing changed yet when I run the solver, the problem persists.)

Originally Posted by Bloerb

zeroGradient on all patches for p_rgh and fixedValue for temperature at all walls. This can't work. Do i have the correct files?

Yeah, the fixed temperature is intentionally set! In reality, the "ACC region" is an activated char coal textile, which is electrically heated on constant ~250°C. Therefore I considered the ACC region isothermal and used fixedValue. Additionally I placed fixedTemperature in fvOptions. Was that a wrong approach?

[jherb]

Originally Posted by ThunderstruckGER

Hey Bloerb, thanks for your reply!
Apart from that I accidentally have set the bc of p at the outlet in the nitrogen region as calculated. I changed that to fixedValue now. (Nothing changed yet when I run the solver, the problem persists.)

This does not make sense: Leave p at calculated and set a fixed value for p_rgh

[ThunderstruckGER]

Originally Posted by jherb

This does not make sense: Leave p at calculated and set a fixed value for p_rgh

Thanks, I have corrected that!

Additionally I deleted all comments in my code, removed wildcards as user Bloerb suggested and checked all bc again with the aid of the multiRegionHeater tutorial case. However, this did not have any impact on the error message.

But, after a lot of trial and error and multiple dead ends, I was able to eventually solve my problem!

As I suggested in my original post, my mistake was very stupid.

The optional settings "thicknessLayers" and "kappaLayers" in the boundary conditions of my solids were set at zero - instead of deleting them from the code. This resulted in the "nan/not a number" problem when the solver tried to calculate the enthalpy of the solids.

[ThunderstruckGER]

Hey everyone,

After the problem leading to the simulation crashing has been corrected, I've run into a few other problems.

The solver was able to calculate ~60 seconds and then failed (timesteps of the calculation got as small as e-12 seconds @ maxCo=1) due to a problem with the boundary conditions in the "air"-region. The "air"-region's purpose is to model the convection of the ambient air outside of my cylinder. I managed to solve that by setting the boundary conditions of p_rgh to fixedFluxPressure instead of fixedValue. Yet, the solver needs 1000 iterations in that region for p_rgh which seems quite high to me and slows down the simulation. Am I still wrong about the boundary conditions in that region, or is that the correct way to set them? Anyways, the solver is now able to calculate the needed 600 seconds without crashing!

Then, another problem emerged when I looked into the temperatures. Not a single region is heating up somewhat realistically. The "nitrogen"-region reached about 310-370K after 600 seconds. The temperature itself is already absurdly low, since the nitrogen is flowing through the "ACC"-region, which is set at fixed 523K. But also, the temperature gap between the cells is way too high and does not make any sense. The "coating"-region heated up to about 310K, but nothing at all happened at the other regions.

I tried setting the boundary conditions for T in the "nitrogen"-region on a value of 523K, sort of as if the module was preheated. By doing this, I also tried to rule out the possibility of the fluid-fluid boundary to be the source of the problem. This lead to the internal field of the "coating"-region heating up more realistically, but "steel" and "air" are still left at constant 300K. I have no idea if what I did there is even physically reasonable, or complete nonsense. But, obviously it does not thermophysically make sense to apply that "workaround" to the other regions, too. So I'm kinda stuck with this problem.

I have tried analyzing my files again and compared them to the tutorial case. I can't find any obvious mistakes and got no approach how to solve this. First, I was so happy to see the simulation running. But upon closer look, this seems to be a train wreck of a simulation

I've uploaded the complete case files of the two versions mentioned above here. Maybe you could take a look into them?

Again, thanks in advance. I would appreciate any help!

Edit

I think it's worth mentioning that the following temperature output is given at the steel_to_coating boundary for the latest timestep. Maybe you have an idea why this is happening.

steel_to_coating
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        refValue        nonuniform List<scalar> 
50
(
345.19299
399.5114
403.97051
412.30316
364.06796
330.25678
328.39206
328.94288
332.58578
342.03977
333.59269
330.2005
331.30204
334.51619
345.02305
338.01482
334.37978
335.07695
338.7749
349.22986
342.0182
337.32768
337.38229
341.38834
352.46732
346.17461
340.18645
339.75424
343.70123
355.47383
351.1891
343.74118
342.71983
346.68532
359.12619
357.43231
348.05081
346.20291
350.36067
363.75169
364.87789
353.19016
350.29909
354.73818
369.1634
373.10082
359.99065
356.20266
360.56087
374.82201
)
;
        refGradient     uniform 0;
        valueFraction   nonuniform List<scalar> 
50
(
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
1.4977913e-05
1.49789e-05
1.4979223e-05
1.49789e-05
1.4977913e-05
)
;
        value           nonuniform List<scalar> 
50
(
300.27603
300.5203
300.57291
300.58401
300.37779
300.16858
300.17517
300.18128
300.20014
300.23294
300.17702
300.16416
300.16942
300.19036
300.23892
300.19955
300.18421
300.18798
300.21092
300.2603
300.22119
300.20098
300.2016
300.2257
300.27789
300.24386
300.21758
300.21526
300.23927
300.29458
300.27133
300.23799
300.23219
300.25634
300.31486
300.30573
300.263
300.25249
300.27752
300.34056
300.34726
300.29316
300.27677
300.30295
300.37102
300.39225
300.33009
300.30859
300.33419
300.40263
)
;
        Tnbr            T;
        thicknessLayers List<scalar> 1(0.001);
        kappaLayers     List<scalar> 1(0.0005);
        kappaMethod     solidThermo;
        kappa           none;
        alphaAni        Anialpha