|
[Sponsors] |
rhoSimpleFoam vs rhoPimpleFoam, steady state vs transient solver |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 21, 2022, 07:59 |
|
#21 |
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 742
Rep Power: 14 |
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). |
|
June 22, 2022, 18:53 |
|
#22 |
New Member
Join Date: May 2018
Posts: 18
Rep Power: 8 |
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. |
|
June 23, 2022, 04:51 |
|
#23 |
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 742
Rep Power: 14 |
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. |
|
July 1, 2022, 07:45 |
|
#24 | |
New Member
Join Date: May 2018
Posts: 18
Rep Power: 8 |
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:
|
||
July 4, 2022, 11:19 |
|
#25 | |
New Member
Join Date: May 2018
Posts: 18
Rep Power: 8 |
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:
|
||
July 4, 2022, 11:22 |
|
#26 |
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 742
Rep Power: 14 |
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.
|
|
January 11, 2023, 08:24 |
|
#27 | |
Member
Anders Aamodt Resell
Join Date: Dec 2021
Location: Oslo, Norway
Posts: 66
Rep Power: 5 |
Quote:
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? |
||
January 11, 2023, 11:28 |
|
#28 |
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 742
Rep Power: 14 |
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. |
|
January 12, 2023, 05:13 |
|
#29 |
Member
Anders Aamodt Resell
Join Date: Dec 2021
Location: Oslo, Norway
Posts: 66
Rep Power: 5 |
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. |
|
Tags |
rhopimplefoam, rhosimplefoam, steady state, transient |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
From steady state to transient simulation | Mechand | FLUENT | 0 | December 24, 2020 13:17 |
Will the results of steady state solver and transient solver be same? | carye | OpenFOAM Running, Solving & CFD | 9 | December 28, 2019 06:21 |
Effect of initial condition for steady state vs Transient | prasa | ANSYS | 0 | August 22, 2018 05:45 |
accelarate simulation using steady state solver | tjliang | OpenFOAM Running, Solving & CFD | 0 | October 7, 2016 15:42 |
Constant velocity of the material | Sas | CFX | 15 | July 13, 2010 09:56 |