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

rhoSimpleFoam vs rhoPimpleFoam, steady state vs transient solver

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

Like Tree10Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 21, 2022, 06:59
Default
  #21
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 667
Rep Power: 14
Tobermory will become famous soon enough
No problem!

My upStream patch is on the upstream end of the "nozzle" - ie the far left vertical boundary in the plots. The downStream patch is to the right of the edge of the picture (only part of the domain is plotted).
Tobermory is offline   Reply With Quote

Old   June 22, 2022, 17:53
Default
  #22
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
Thank you again for your answer!

I assume your geometry looks somehow like this?

And do you use a mass flow rate or just a normal velocity bc for the inlet?

I have also seen the T limit method in the aerofoil tutorial, but is there a reason why you limit the temperature not the rho?

To be able to avoid a unsteady solver would be a rescue for me, since i have been trying this for months. So please forgive me if i ask too specifically and too much.

Quote:
Originally Posted by Tobermory View Post
No problem!

My upStream patch is on the upstream end of the "nozzle" - ie the far left vertical boundary in the plots. The downStream patch is to the right of the edge of the picture (only part of the domain is plotted).
Attached Images
File Type: jpg Bildschirmfoto 2022-06-22 um 23.46.08.jpg (32.3 KB, 34 views)
Oliver Meng is offline   Reply With Quote

Old   June 23, 2022, 03:51
Default
  #23
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 667
Rep Power: 14
Tobermory will become famous soon enough
Yes - that's right. I am specifying the (total) pressure on the upstream boundary, so I have a zeroGradient BC on U ... you can't specify both p & U since that overconstrains the problem. On the downstream boundary I have a fixed pressure and a pressureInletOutletVelocity for U (i.e. zerogradient).

As for limiting - it's simpler for me to limit T since I know a-priori what the range will be, and keeping a tight control on T stops the Janaf class going nuts with temperature out of range errors (when calculating Cp). I guess there's no reason why you couldn't limit rho instead, although I haven't tried it - you'd need to check that the rho equation in your solver allows for fvOptions.

One other thing - again related to stability - I start by running with basic kEpsilon, and get a converged solution, before changing over to realizableKE, which is much less stable but gives a far better, less diffusive solution.

Again - good luck, and I hope that some of the above helps.
Tobermory is offline   Reply With Quote

Old   July 1, 2022, 06:45
Default
  #24
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
I have been struggling with this problem for another week and again without success. Supersonic with steady solver is kinda annoying. But since i'm only interested in the force coefficient, it is really not necessary to use a transient solver for any time related values.

My case is 3D but a 2D slice also tells the story and it looks like this.(attachment)

The flow will choke at the “bottleneck” and rise after that.

Since my domain is quite small I used k-omega-SST to also (trying to) get a good result in the near wall region.
My inlet has a velocity condition and outlet fixed pressure.
Inspired by you I’m gonna try to increase my inlet velocity step by step (like you total pressure) from 40 to 100 m/s and see if it helps.

Regards

Quote:
Originally Posted by Tobermory View Post
Yes - that's right. I am specifying the (total) pressure on the upstream boundary, so I have a zeroGradient BC on U ... you can't specify both p & U since that overconstrains the problem. On the downstream boundary I have a fixed pressure and a pressureInletOutletVelocity for U (i.e. zerogradient).

As for limiting - it's simpler for me to limit T since I know a-priori what the range will be, and keeping a tight control on T stops the Janaf class going nuts with temperature out of range errors (when calculating Cp). I guess there's no reason why you couldn't limit rho instead, although I haven't tried it - you'd need to check that the rho equation in your solver allows for fvOptions.

One other thing - again related to stability - I start by running with basic kEpsilon, and get a converged solution, before changing over to realizableKE, which is much less stable but gives a far better, less diffusive solution.

Again - good luck, and I hope that some of the above helps.
Attached Images
File Type: jpg screenshot.jpg (16.4 KB, 18 views)
Oliver Meng is offline   Reply With Quote

Old   July 4, 2022, 10:19
Default
  #25
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
Hi,

after trying with different tricks and methods, i still did not get it converged.

Do you happen to know, or do you have experience, if the steady state solver for compressible flow in Ansys is more stable for a supersonic flow compared to Openfoam?

Regards

Quote:
Originally Posted by Tobermory View Post
Yes - that's right. I am specifying the (total) pressure on the upstream boundary, so I have a zeroGradient BC on U ... you can't specify both p & U since that overconstrains the problem. On the downstream boundary I have a fixed pressure and a pressureInletOutletVelocity for U (i.e. zerogradient).

As for limiting - it's simpler for me to limit T since I know a-priori what the range will be, and keeping a tight control on T stops the Janaf class going nuts with temperature out of range errors (when calculating Cp). I guess there's no reason why you couldn't limit rho instead, although I haven't tried it - you'd need to check that the rho equation in your solver allows for fvOptions.

One other thing - again related to stability - I start by running with basic kEpsilon, and get a converged solution, before changing over to realizableKE, which is much less stable but gives a far better, less diffusive solution.

Again - good luck, and I hope that some of the above helps.
Oliver Meng is offline   Reply With Quote

Old   July 4, 2022, 10:22
Default
  #26
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 667
Rep Power: 14
Tobermory will become famous soon enough
That must be really frustrating. I don't have any recent experience with Ansys Fluent or CFX ... my recollection is that StarCCM+ was more stable, but I do not have access to that at the moment.
Tobermory is offline   Reply With Quote

Old   January 11, 2023, 07:24
Default
  #27
Member
 
Anders Aamodt Resell
Join Date: Dec 2021
Location: Oslo, Norway
Posts: 64
Rep Power: 4
ander is on a distinguished road
Quote:
Originally Posted by arjun View Post
the idea that if the solver is unstable than it must be more accurate compared to stable solver is completely not true.

It is more so not true when you compare OF against StarCCM. CCM does not add sort of artifical dissipation to make it stable and not only that its descretization is actually more accurate.

I personally have never found a case where starccm and of are compared and starccm came out to be less accurate.

Mostly if you benchmark you will find that starccm does better than OF.

I even have a study where most scheme of OF for convection terms were compared in a validation case and starccm was also one of the solver. Guess what there was hardly any scheme that was as good as starccm and around 40 scheme were compared.

Give me email i will send you the results.
Dear Arjun,

This was suprising to me as well as I've long had the impression that commercial solvers use artificial diffusion or similar techniques to increase robustness. This is for instance championed by this post: https://www.linkedin.com/pulse/accur...s-lubos-pirkl/

Could you eloborate on what starccm+ does to be both robust and accurate at the same time. Or is the idea that comemrcial solvers are more robust simply a myth?
ander is offline   Reply With Quote

Old   January 11, 2023, 10:28
Default
  #28
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 667
Rep Power: 14
Tobermory will become famous soon enough
It's not a myth - they really are more robust (at least StarCCM+ is), and the article/blog that you linked (a really good read - thanks!) explains why - commercial reality in essence.

It's still possible to make a StarCCM+ simulation explode (I am running various cases at the moment) ... but usually only if you make a big mistake with the boundary condition or initial field setup. Sadly, that's not the case with OpenFOAM.

There are a bunch of limiters and the like in StarCCM+ - many of which you can adjust or turn off (eg rough wall limiter, turb viscosity limiter), but I suspect that some of the magic (ie source of robustness) is in the boundary condition coding, which of course is not open for scrutiny or adjustment in a commercial code.
Tobermory is offline   Reply With Quote

Old   January 12, 2023, 04:13
Default
  #29
Member
 
Anders Aamodt Resell
Join Date: Dec 2021
Location: Oslo, Norway
Posts: 64
Rep Power: 4
ander is on a distinguished road
I think there is a slight mismatch between what that linkedinpost conveyed (that you can have either robustness or accuracy) and what Arjun reported (that you can have both).

If starccm+ is indeed accurate and robust and the same time, it really is superior compared to opensource. A shame that the methods used by these companies to increase robustness aren’t public knowledge.
ander is offline   Reply With Quote

Reply

Tags
rhopimplefoam, rhosimplefoam, steady state, transient

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
From steady state to transient simulation Mechand FLUENT 0 December 24, 2020 12:17
Will the results of steady state solver and transient solver be same? carye OpenFOAM Running, Solving & CFD 9 December 28, 2019 05:21
Effect of initial condition for steady state vs Transient prasa ANSYS 0 August 22, 2018 04:45
accelarate simulation using steady state solver tjliang OpenFOAM Running, Solving & CFD 0 October 7, 2016 14:42
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56


All times are GMT -4. The time now is 04:26.