PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Forum rules
Please read the forum usage recommendations before posting.
Please read the forum usage recommendations before posting.
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Dear Yvan, if you change the time step from 0.001 to 1.0e-6 the simulation will run on v5.0.4 as verified by attached animation video which I made with the latest xml input from Christopher edited ONLY on the time step setting. The video shows the first 50 time steps of 1.e-6 - long enough to show a healthy propagation of the disturbance from the suddenly applied inlet flow.
- Attachments
-
- Exxon_III.ogv.zip
- (162.52 KiB) Downloaded 158 times
-
- Posts: 4082
- Joined: Mon Feb 20, 2012 3:25 pm
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Hello,
I am able to run the case with the smaller time step on all releases of v5.0, up to v5.0.13, but this is broken by my patch for incorrect BC handling by the GUI. I will need to investigate further, but I guess that using the full BC's leads to steeper boundary conditions, because that patch should be used to get consistent BC's (at least, BC's as expected).
I'll keep you informed.
Best regards,
Yvan
I am able to run the case with the smaller time step on all releases of v5.0, up to v5.0.13, but this is broken by my patch for incorrect BC handling by the GUI. I will need to investigate further, but I guess that using the full BC's leads to steeper boundary conditions, because that patch should be used to get consistent BC's (at least, BC's as expected).
I'll keep you informed.
Best regards,
Yvan
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Dear Yvan.
Thank you very much. It is highly appreciated.
Thank you very much. It is highly appreciated.
-
- Posts: 36
- Joined: Wed Feb 17, 2021 2:22 pm
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Hello,
that is interesting.
tpa, the simulation result looks pretty good. I also tried smaller time steps. However, it did not work in code_saturne 5.3? Even if I use your XML with variable time stepping. It is astonishing, that it works properly in previous versions.
Yvan, do you think it will work in 6.0? Maybe I should figure out how to update my version to 6.0. As mentioned earlier, I use CAE Linux 2020 with Salome using the CFDSTUDY module. Or maybe it is better to use a clean installation of code_saturne outside of Salome?
Thank you.
Best regards,
Christopher
that is interesting.
tpa, the simulation result looks pretty good. I also tried smaller time steps. However, it did not work in code_saturne 5.3? Even if I use your XML with variable time stepping. It is astonishing, that it works properly in previous versions.
Yvan, do you think it will work in 6.0? Maybe I should figure out how to update my version to 6.0. As mentioned earlier, I use CAE Linux 2020 with Salome using the CFDSTUDY module. Or maybe it is better to use a clean installation of code_saturne outside of Salome?
Thank you.
Best regards,
Christopher
-
- Posts: 4082
- Joined: Mon Feb 20, 2012 3:25 pm
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Hello,
I will test your case on a more recent version, but on my machine, it is the bug fix which causes the negative density values and subsequent stop. I suspect the boundary conditions are too steep for the initialization, but am not sure yet.
So things might be better in v6.0.6 (without the bug fix) or similar, but we will probably have the same issue after that.
I'll look at why the density becomes negative in some cells in a few days at most and keep you informed.
Best regards,
Yvan
I will test your case on a more recent version, but on my machine, it is the bug fix which causes the negative density values and subsequent stop. I suspect the boundary conditions are too steep for the initialization, but am not sure yet.
So things might be better in v6.0.6 (without the bug fix) or similar, but we will probably have the same issue after that.
I'll look at why the density becomes negative in some cells in a few days at most and keep you informed.
Best regards,
Yvan
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
My recommendation to You, Christopher, is to acquire a version v5.0.4 because that seems to work. As you can see from the other thread I tested several versions, including present v5.3 (Salome_CFD) and v6 and v7 (from github)which all failed to run. Unless, of course you want to try for yourself, which would also be respected.
If You can not obtain the codebase for v5.0.4 elsewhere You can have a copy from me.
If You can not obtain the codebase for v5.0.4 elsewhere You can have a copy from me.
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
While reflecting on your case ... What is your thinking about the difference between having symmetry boundary conditions on the top and bottom versus having walls as you have now?
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Dear Christopher and Yvan.
Since this seems the opportunity to promote getting functionality back into the compressible module I have made another run with the case. Based on the most recent xml file provided by Christopher except for the time settings.
Yvan - Regarding negative energy error, It IS related to time stepping. It is clearly stated in the manual that Courant numbers should be limited to 0.4. For a fine mesh this WILL mean small timesteps.
For this run I used constant time stepping of 5e-07 seconds asked for 20000 timesteps (10ms total) and left the computer running overnight. This timestep will just fulfill the recommendation of CFL<0.4 for the full domain over all time steps.
For your consideration I have generated 2 new videos for the case. Exxon_IV shows the development in Mach number and Exxon_V shows the jet formation outside the nozzle. All looks pretty good to me,
You still need an older Code_Saturne - like my v5.0.4 to complete such simulations. I cross my fingers that it will be possible in future releases again.
Since this seems the opportunity to promote getting functionality back into the compressible module I have made another run with the case. Based on the most recent xml file provided by Christopher except for the time settings.
Yvan - Regarding negative energy error, It IS related to time stepping. It is clearly stated in the manual that Courant numbers should be limited to 0.4. For a fine mesh this WILL mean small timesteps.
For this run I used constant time stepping of 5e-07 seconds asked for 20000 timesteps (10ms total) and left the computer running overnight. This timestep will just fulfill the recommendation of CFL<0.4 for the full domain over all time steps.
For your consideration I have generated 2 new videos for the case. Exxon_IV shows the development in Mach number and Exxon_V shows the jet formation outside the nozzle. All looks pretty good to me,
You still need an older Code_Saturne - like my v5.0.4 to complete such simulations. I cross my fingers that it will be possible in future releases again.
- Attachments
-
- Exxon_V.ogv.zip
- (4.61 MiB) Downloaded 147 times
-
- Exxon_IV.ogv.zip
- (277.84 KiB) Downloaded 150 times
-
- Posts: 4082
- Joined: Mon Feb 20, 2012 3:25 pm
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Hello,
Thanks for the feedback. I have not tested this on v6 yet, but had it working with small time steps even up to 5.0.12. So the difference in behavior is strange.
I'll get back to this in a few days, after I am finished with another feature which needs to be in v7.0. What I would like to do is to try to make the behavior more robust, perhaps "clipping" impossible (negative) values so as to at least not crash with higher time steps, even though better precision will still require smaller time steps. This could accelerate convergence.
Best regards,
Yvan
Thanks for the feedback. I have not tested this on v6 yet, but had it working with small time steps even up to 5.0.12. So the difference in behavior is strange.
I'll get back to this in a few days, after I am finished with another feature which needs to be in v7.0. What I would like to do is to try to make the behavior more robust, perhaps "clipping" impossible (negative) values so as to at least not crash with higher time steps, even though better precision will still require smaller time steps. This could accelerate convergence.
Best regards,
Yvan
Re: PROBLEM IN THE BOUNDARY CONDITIONS USING COMPRESSABLE MODEL
Dear Yvan,
Thank you for having attention on this.
Ad 1 - Robustness/convergence
In my understanding unsteady solutions to flow analysis do not converge unless the model - i.e. combination of fluid domain, boundary conditions and fluid properties allows it to so to say. To me the most important thing is to be able to run the analysis at all, not so much optimizing aspect.
Ad 2 - Disappearing boundary conditions
This is the primary issue to solve before CS will solve a compressible study. Below is a part of the v5.0.4 listing from the first time step. Under the heading " ** BOUNDARY MASS FLOW INFORMATION" you can see that the mass flow has been transferred correctly. If you look at the simlilar lines from the newer versions the "Imp inlet/outlet" is most likely zero.
If You look at the corresponding lines of one of my tests with v6.3.0 (below) it reads all zeros. This was a different model so the number of faces are different, but the issue IS there.
In v5.0(.4) mass flow was correctly transferred and the analysis ran perfectly well as can be seen in this thread: viewtopic.php?f=12&t=2801
There may be other issues, but this exact issue can be seen directly in the listing - so thank you for keeping the listing so detailed
Thank you for having attention on this.
Ad 1 - Robustness/convergence
In my understanding unsteady solutions to flow analysis do not converge unless the model - i.e. combination of fluid domain, boundary conditions and fluid properties allows it to so to say. To me the most important thing is to be able to run the analysis at all, not so much optimizing aspect.
Ad 2 - Disappearing boundary conditions
This is the primary issue to solve before CS will solve a compressible study. Below is a part of the v5.0.4 listing from the first time step. Under the heading " ** BOUNDARY MASS FLOW INFORMATION" you can see that the mass flow has been transferred correctly. If you look at the simlilar lines from the newer versions the "Imp inlet/outlet" is most likely zero.
Code: Select all
INSTANT 0.500000000E-06 TIME STEP NUMBER 1
=============================================================
-----------------------------------------
Property Min. value Max. value
-----------------------------------------
density 0.1204E+01 0.1204E+01
molecular_viscos 0.2835E-04 0.2835E-04
turbulent_viscos 0.9202E-03 0.9202E-03
-----------------------------------------
--- Diffusivity:
-----------------------------------------------
Scalar Number Min. value Max. value
-----------------------------------------------
TotEner 1 0.5544E-04 0.5544E-04
temperature 2 0.4164E-01 0.4164E-01
-----------------------------------------------
** INFORMATION ON BOUNDARY FACES TYPE
----------------------------------
-------------------------------------------------------------------------
Boundary type Code Nb faces
-------------------------------------------------------------------------
Sub. enth. inlet 11 0
Ptot, Htot 10 0
Imp inlet/outlet 7 216
Subsonic outlet 9 346
Supersonic outlet 8 0
Smooth wall 5 1464
Rough wall 6 0
Symmetry 4 149592
Undefined 1 0
-------------------------------------------------------------------------
** BOUNDARY MASS FLOW INFORMATION
------------------------------
---------------------------------------------------------------
Boundary type Code Nb faces Mass flow
---------------------------------------------------------------
Sub. enth. inlet 11 0 0.000000000E+00
Ptot, Htot 10 0 0.000000000E+00
Imp inlet/outlet 7 216 0.193111033E-01
Subsonic outlet 9 346 0.000000000E+00
Supersonic outlet 8 0 0.000000000E+00
Wall 5 1464 0.000000000E+00
Symmetry 4 149592 0.000000000E+00
Undefined 1 0 0.000000000E+00
---------------------------------------------------------------
Code: Select all
** BOUNDARY MASS FLOW INFORMATION
------------------------------
---------------------------------------------------------------
Boundary type Code Nb faces Mass flow
---------------------------------------------------------------
Sub. enth. inlet 11 0 0.000000000E+00
Ptot, Htot 10 562 0.000000000E+00
Imp inlet/outlet 7 93 0.000000000E+00
Subsonic outlet 9 985 0.000000000E+00
Supersonic outlet 8 0 0.000000000E+00
Wall 5 3728 0.000000000E+00
Symmetry 4 0 0.000000000E+00
Undefined 1 0 0.000000000E+00
---------------------------------------------------------------
There may be other issues, but this exact issue can be seen directly in the listing - so thank you for keeping the listing so detailed