CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Transonic Diffuser Case: Floating Point Exception

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree10Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 18, 2018, 19:04
Default
  #21
Senior Member
 
Peter Hess
Join Date: Apr 2011
Location: Austria
Posts: 250
Rep Power: 16
peterhess is on a distinguished road
Hello Saleh!

Try those setups.

https://drive.google.com/file/d/1PnR...ew?usp=sharing

I had a good convergence for more than 10000 iterations.

Regards

Peter

Last edited by peterhess; December 18, 2018 at 21:43.
peterhess is offline   Reply With Quote

Old   December 18, 2018, 23:21
Default
  #22
Member
 
Fatih Ertinaz
Join Date: Feb 2011
Location: Istanbul
Posts: 64
Rep Power: 15
fertinaz is on a distinguished road
Hello Peter and Saleh

I checked this case as well if you don't mind.

Since both solvers fail during the pressure correction evaluation, I focused on the pressure first. I applied Robin BC at the inlet:
Code:
    Inlet
    {
        type            zeroGradient;
        refValue        uniform 116800;
        refGradient     uniform 0;
        valueFraction   uniform 0.1;

        // type            fixedValue;
        // value           uniform 116800;
    }
It initially worked fine but then I realized that blow-up was just delayed.

Then I took a look at the "system/fvSolution" and modified:
Code:
    rhoMin        0.1;
    rhoMax        2;
and also reduced the pressure relaxation to 0.7. Not sure if 1 is a good value which will chop-off the deviations for stability but may produce unphysical results.

These modifications let simulations run even further but could not prevent blow-up which this time occurred at "Time = 0.4597".

Therefore I changed velocity outlet to kill potential inward reflections on the outlet patch:
Code:
    Outlet
    {
        type            inletOutlet;
        inletValue      uniform (150.6 0 0);
        value           $internalField;

        // type            zeroGradient;
    }
It now seems to run fine. It already passed "Time = 3.3" with "deltaT 1e-04;".

Please test it and see if it works for you as well.

I'd highly recommend you to check the last few steps prior to the blow-ups and try to see why they occur. Visualising may help you out.

// Fatih
peterhess and Saleh Abuhanieh like this.
fertinaz is offline   Reply With Quote

Old   December 18, 2018, 23:34
Default
  #23
Member
 
Saleh Abuhanieh
Join Date: Nov 2017
Posts: 82
Rep Power: 8
Saleh Abuhanieh is on a distinguished road
Gunaydin Fatih,


Thanks for your contribution, I'll run with your suggestions and get back to you.


Saleh

Regards,
Saleh Abuhanieh is offline   Reply With Quote

Old   December 19, 2018, 12:47
Default
  #24
Senior Member
 
Peter Hess
Join Date: Apr 2011
Location: Austria
Posts: 250
Rep Power: 16
peterhess is on a distinguished road
Hello Fatih and Saleh!

I tested the suggestions you made (on the case I uploaded lately with the turbulence activated) and they works!

You get convergence very nice and the results are for me have physical meaning...

-------------------------

The last sugesstion is helping the simulation getting convergence. The simulation does not have back flow, anyway, It increase the stability.

I would also do it this way...

-------------------------

The secound suggetion is already applied cause the density at the inlet is higher than 1.05...

-------------------------

The first suggestion is solving the problem!

Anyway, The pressure at the inlet is not fixed anymore as Saleh already confirmed to be!

The problem here is that Saleh is fixing the pressure at the inlet and the outlet and at the same time fixing the velocity at the inlet...

That is physicaly (in my opinion and I may be wrong) not applicable...

Eather you fix the "statical" pressure at the inlet and the outlet and look for the velocity driven via pressure difference.

Or you fix the velocity at the inlet and the "statical" pressure at the outlet and then see which pressure is needed at the inlet to force this pre defined velocity.

The suggestion of Fatih is somehow in this direction.

The simulation as it has been setuped by Saleh is "over defined" in my opinion.

I would define the pressure at the inlet as totalPressure and let the simulation divide it (calculate) between velocity and static pressure.

----------------------------

Saleh: I looked to the paper you mentioned earlier.

The pressure at the inlet is NOT statical.

It is totalPressure

See page 57 (68/100) - table 4-2 - inflow!

Benjamin actualy mentioned on the same page at the bottom that the pressure is fixed at the inlet, but he did not say it is statical! He means fixed totalPressure

Cause on the next page - Figure 4.11 - a, the pressure everywhere is less than the pressure you defined to be "statical" fixed at the inlet.

Regards

Peter
Saleh Abuhanieh likes this.

Last edited by peterhess; December 20, 2018 at 01:30.
peterhess is offline   Reply With Quote

Old   December 20, 2018, 10:33
Default
  #25
Member
 
Saleh Abuhanieh
Join Date: Nov 2017
Posts: 82
Rep Power: 8
Saleh Abuhanieh is on a distinguished road
Dear Peter and Fatih,


Thank you very much for your support!


I've been running the latest case (the uploaded cases from Peter with Fatih's comments). The residual is quite smooth and in the range of 1e0-5 now and the flow is not changing any more. I attached the velocity profile at 183k iteration, the result still different from the original case (Benjamin's) and there is big difference in the max velocity (270 m/s comparing 498 m/s). I stopped at 205k iteration, complete convergence.







Yes Peter, I agree with you that the case became over-defined!
Thank you for referring to the original work and your valuable comments.

Actually as I highlighted earlier in this thread, I think the problem some where in the BC. I tried before using totalPressure at the inlet, but I got FPE as well, this is why I left it static (as per my wrong interpretation for Benjamen's words).


Starting from the initial case uploaded by me with changing only the inlet BC to totalPressure, I got FPE at around 14k iteration and the residual is fluctuating.



Time = 13801

smoothSolver: Solving for Ux, Initial residual = 0.000258627, Final residual = 2.31127e-05, No Iterations 10
smoothSolver: Solving for Uy, Initial residual = 0.000332803, Final residual = 3.06775e-05, No Iterations 8
smoothSolver: Solving for e, Initial residual = 0.000239535, Final residual = 1.70034e-05, No Iterations 6
GAMG: Solving for p, Initial residual = 0.000125527, Final residual = 1.57558e-06, No Iterations 1
time step continuity errors : sum local = 620.309, global = -309.237, cumulative = -4.36703e+06
ExecutionTime = 964.21 s ClockTime = 965 s

Time = 13802

smoothSolver: Solving for Ux, Initial residual = 0.000301733, Final residual = 2.6563e-05, No Iterations 28
smoothSolver: Solving for Uy, Initial residual = 0.000354937, Final residual = 3.09186e-05, No Iterations 18
smoothSolver: Solving for e, Initial residual = 0.0118356, Final residual = 0.000707792, No Iterations 10
GAMG: Solving for p, Initial residual = 0.000130643, Final residual = 1.77223e-06, No Iterations 1
time step continuity errors : sum local = 637.933, global = -309.221, cumulative = -4.36734e+06
ExecutionTime = 964.3 s ClockTime = 965 s

Time = 13803

smoothSolver: Solving for Ux, Initial residual = 0.00349629, Final residual = 0.000234674, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.00126557, Final residual = 0.000109374, No Iterations 2
smoothSolver: Solving for e, Initial residual = 0.0243903, Final residual = 0.00210812, No Iterations 2




I'll try now the uploaded case by peter with Fatih's comments with changing the inlet BC and post the results.


Regards,

Saleh
Attached Images
File Type: png mag(U)_at_183k_iteration.png (20.1 KB, 5 views)
Saleh Abuhanieh is offline   Reply With Quote

Old   December 25, 2018, 11:09
Default
  #26
Member
 
Saleh Abuhanieh
Join Date: Nov 2017
Posts: 82
Rep Power: 8
Saleh Abuhanieh is on a distinguished road
Hi Foamers,


I just wanted to give a feedback about the case for reference.
Using the totalPressure BC at the inlet produces a stable results but not accurate and far from the reference study which was based on sonicTurboFoam and experimental resluts.


With the same setup, only reducing the time step to 1e-06, I got a good results using sonicFoam.

Then I tried the same for the other two cases in the reference thesis, namely: the weak and strong shock, however I didn't get acceptable results (the velocity is too lower). When I changed the inlet BC to fixedValue (@peter ), The results were acceptable; more accurate in case of weak shock and less accurate in case of strong shock.


Regards,
Saleh Abuhanieh is offline   Reply With Quote

Old   April 8, 2023, 06:55
Default
  #27
New Member
 
Alessio Piccolo
Join Date: May 2022
Location: Italy
Posts: 9
Rep Power: 3
Ale22pic is on a distinguished road
Hi everybody, I know it is been a while. But it is possible to have the transonic diffuser test case. I'm struggling to solve it with rhoCentralFoam in Openfoam, unfortunately the links in this thread don't work anymore. Thank you in advance.
Ale22pic is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Floating point exception in tutorials case xujr OpenFOAM Running, Solving & CFD 0 May 21, 2015 04:31
Floating point exception (core dumped) in transonicMRFDyMFoam sam.ho OpenFOAM Running, Solving & CFD 0 April 29, 2014 02:30
interDyMFoam- Floating point exception Error marhamat OpenFOAM Running, Solving & CFD 2 December 26, 2012 14:40
[Gmsh] Gmsh and samplesurface touf OpenFOAM Meshing & Mesh Conversion 2 December 10, 2007 03:27
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 13:24


All times are GMT -4. The time now is 20:12.