Unable to validate results with sonicFoam and rhoCentralFoam

lordvon · June 9, 2016, 17:15

What I thought was going to be a simulation of trivial physics, was in fact something the supersonic solvers in OpenFOAM could not handle. I was trying to validate an axisymmetric simulation of a converging-diverging nozzle with the data found here:

http://www.grc.nasa.gov/WWW/wind/valid/cdv/cdv.html

The pressure ratio of 0.89 (subsonic, peaking at 0.8+ Mach) simply could not match; peaks were much too low by about 10%, when it should be almost exactly matching. I tried different numerical schemes, grid resolutions, to no avail. The pressure ratio of 0.16 (supersonic, no shocks in throat) actually predicted a shock right at the exit, causing the predicted pressures to be much too high and the Mach numbers much too low.

So you can observe this for yourself, the boundary condition directories that I used can be found in 'case_sonic/0' and 'case_rhocentral/0' at the following github page:

https://github.com/rlee32/upcoming/tree/master/CDNozzle

Let me know what you think...

[Moderator note: For future reference, the original title was: PSA: sonicFoam and rhoCentralFoam are bunk...]

wyldckat · June 18, 2016, 17:57

Quick note: I haven't checked the case set-up you have (and this topic is beyond my expertises

), but there have been others who have stumbled on this issue. A few examples:

http://www.cfd-online.com/Forums/ope...-aerofoam.html
I can't remember exactly if it was the forum member skeptik who had this issue as well or not: http://www.cfd-online.com/Forums/blogs/skeptik/

schuyler · July 14, 2016, 15:00

My experience with rhoCentralFoam has been very positive! I believe the problem you are experiencing is due to your setup. I think the main issue is that the totalPressure boundary condition requires a definition of psi for compressible flow.

Since this is a compressible flow the definition of psi should be

Code:

thermo:psi

calling psi from the thermophysical models set for the compressible flow.

With regards to the supersonic flow with an unwanted shock, you should not specify an outlet pressure for this case. You CAN. But remember that the supersonic flow solution for this problem is unique (contrasting to flow with shock, or subsonic where the solution is not unique). It does not require this information. All you are doing is making the simulation more rigid. Unless you input the exact answer that the solver is looking for (and this will depend slightly on schemes, resolution etc) you will have some difficulties. The shock formed because of this probably. I suggest using zeroGradient for the outlet pressure. Once you get the answer, how closely the exit pressure matches the analytical, expected result, will be an indication of the quality of the solution.

I started a blog on CFD about 6 months ago. I just made a post regarding this test case:

https://curiosityfluids.com/2016/07/...hocentralfoam/

I am still building up the content. But now this case is covered! Hopefully this helps.

lordvon · July 15, 2016, 23:36

Great job schuyler! I wish I could change the title now, but it seems I cannot.

blais.bruno · September 1, 2016, 11:03

Dear Schuyler,
Do you have the mesh and files for the tests cases you discuss on your blog post?

Best regards,
Bruno

Quote:

Originally Posted by schuyler

My experience with rhoCentralFoam has been very positive! I believe the problem you are experiencing is due to your setup. I think the main issue is that the totalPressure boundary condition requires a definition of psi for compressible flow.

Since this is a compressible flow the definition of psi should be

Code:

thermo:psi

calling psi from the thermophysical models set for the compressible flow.

With regards to the supersonic flow with an unwanted shock, you should not specify an outlet pressure for this case. You CAN. But remember that the supersonic flow solution for this problem is unique (contrasting to flow with shock, or subsonic where the solution is not unique). It does not require this information. All you are doing is making the simulation more rigid. Unless you input the exact answer that the solver is looking for (and this will depend slightly on schemes, resolution etc) you will have some difficulties. The shock formed because of this probably. I suggest using zeroGradient for the outlet pressure. Once you get the answer, how closely the exit pressure matches the analytical, expected result, will be an indication of the quality of the solution.

I started a blog on CFD about 6 months ago. I just made a post regarding this test case:

https://curiosityfluids.com/2016/07/...hocentralfoam/

I am still building up the content. But now this case is covered! Hopefully this helps.

schuyler · September 2, 2016, 19:11

Hi Bruno,

I will update the blog this weekend and upload the files! I usually do... dont really know why I forgot this time.

Schuyler

Quote:

Originally Posted by blais.bruno

Dear Schuyler,
Do you have the mesh and files for the tests cases you discuss on your blog post?

Best regards,
Bruno

schuyler · September 6, 2016, 18:38

The blog post is updated now with a downloadable link.

Quote:

Originally Posted by blais.bruno

Dear Schuyler,
Do you have the mesh and files for the tests cases you discuss on your blog post?

Best regards,
Bruno

blais.bruno · December 5, 2016, 15:16

Hello!
Thank you very much for putting the files online.
However I have a question. I am trying to reproduce the subsonic and the sonic (well the case where there is a shock wave within the nozzle) and I am getting confusing results. How do you set the pressure outlet boundary? do you set it as a totalPressure boundary condition (specifying thermo

si and etc.) or as a regular pressure BC with fixedValue?

I think I am failing to understand the maths and physics behind the totalPressure BC.
Sorry, I am not too familiar with compressible flows....

Quote:

Originally Posted by schuyler

The blog post is updated now with a downloadable link.

schuyler · December 5, 2016, 15:25

Quote:

Originally Posted by blais.bruno

Hello!
Thank you very much for putting the files online.
However I have a question. I am trying to reproduce the subsonic and the sonic (well the case where there is a shock wave within the nozzle) and I am getting confusing results. How do you set the pressure outlet boundary? do you set it as a totalPressure boundary condition (specifying thermo

si and etc.) or as a regular pressure BC with fixedValue?

I think I am failing to understand the maths and physics behind the totalPressure BC.
Sorry, I am not too familiar with compressible flows....

For the outlet boundary, I set the pressure as a fixedValue. You can see how the outlet pressure dictates the location of a normal shock in a nozzle here:

https://curiosityfluids.com/2016/03/...l-shock-waves/

also, an alternative case to the one discussed in this feed is posted here:

https://curiosityfluids.com/2016/04/...hocentralfoam/

Schuyler

June 9, 2016, 17:15	Unable to validate results with sonicFoam and rhoCentralFoam	#1
lordvon Senior Member Robert Join Date: Sep 2010 Posts: 158 Rep Power: 16	What I thought was going to be a simulation of trivial physics, was in fact something the supersonic solvers in OpenFOAM could not handle. I was trying to validate an axisymmetric simulation of a converging-diverging nozzle with the data found here: http://www.grc.nasa.gov/WWW/wind/valid/cdv/cdv.html The pressure ratio of 0.89 (subsonic, peaking at 0.8+ Mach) simply could not match; peaks were much too low by about 10%, when it should be almost exactly matching. I tried different numerical schemes, grid resolutions, to no avail. The pressure ratio of 0.16 (supersonic, no shocks in throat) actually predicted a shock right at the exit, causing the predicted pressures to be much too high and the Mach numbers much too low. So you can observe this for yourself, the boundary condition directories that I used can be found in 'case_sonic/0' and 'case_rhocentral/0' at the following github page: https://github.com/rlee32/upcoming/tree/master/CDNozzle Let me know what you think... [Moderator note: For future reference, the original title was: PSA: sonicFoam and rhoCentralFoam are bunk...] Last edited by wyldckat; September 9, 2016 at 19:13. Reason: see "Moderator note:"

June 18, 2016, 17:57		#2
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Quick note: I haven't checked the case set-up you have (and this topic is beyond my expertises ), but there have been others who have stumbled on this issue. A few examples: http://www.cfd-online.com/Forums/ope...-aerofoam.html I can't remember exactly if it was the forum member skeptik who had this issue as well or not: http://www.cfd-online.com/Forums/blogs/skeptik/

July 14, 2016, 15:00		#3
schuyler Member W. Schuyler Hinman Join Date: Apr 2013 Location: Calgary, Alberta, Canada Posts: 38 Rep Power: 13	My experience with rhoCentralFoam has been very positive! I believe the problem you are experiencing is due to your setup. I think the main issue is that the totalPressure boundary condition requires a definition of psi for compressible flow. Since this is a compressible flow the definition of psi should be Code: thermo:psi calling psi from the thermophysical models set for the compressible flow. With regards to the supersonic flow with an unwanted shock, you should not specify an outlet pressure for this case. You CAN. But remember that the supersonic flow solution for this problem is unique (contrasting to flow with shock, or subsonic where the solution is not unique). It does not require this information. All you are doing is making the simulation more rigid. Unless you input the exact answer that the solver is looking for (and this will depend slightly on schemes, resolution etc) you will have some difficulties. The shock formed because of this probably. I suggest using zeroGradient for the outlet pressure. Once you get the answer, how closely the exit pressure matches the analytical, expected result, will be an indication of the quality of the solution. I started a blog on CFD about 6 months ago. I just made a post regarding this test case: https://curiosityfluids.com/2016/07/...hocentralfoam/ I am still building up the content. But now this case is covered! Hopefully this helps. Last edited by schuyler; July 14, 2016 at 15:43. Reason: thermo:psi giving smiley face

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Which equations are solved by rhoCentralFoam, rhoSimplecFoam and sonicFoam?	gamma_user	OpenFOAM Verification & Validation	1	April 19, 2015 13:13
sonicFoam vs rhoCentralFoam forwardStep tutorial	hk318i	OpenFOAM Running, Solving & CFD	2	March 12, 2015 12:15
rhoCentralFoam / sonicFoam	VSass	OpenFOAM Running, Solving & CFD	1	June 26, 2013 13:39
is sonicFoam better in convergence than rhoPimplefoam or rhoCentralFoam?	immortality	OpenFOAM Running, Solving & CFD	1	February 11, 2013 23:26

July 15, 2016, 23:36		#4
lordvon Senior Member Robert Join Date: Sep 2010 Posts: 158 Rep Power: 16	Great job schuyler! I wish I could change the title now, but it seems I cannot.