Thank you Antech for the ideas you shared.
I'm planning to make more tests on the basis of your suggestions, when I have enough machine-time. I must also learn how to make good meshes.
Yvan, I made a new experiment, changing the Velocity-Pressure algorithm, from SIMPLEC to SIMPLE and it looks like it is the main responsible for the differences. Even if I wouldn't say that the results converged to a steady state solution, they are much close to the ones obtained with sat2.
simulations comparison
I still need a very long time (about 16 hours) to finish the simulation, which is longer than the time I needed with saturne 2.
Ccaccia73 Some words about meshes for SST. I created them in Mesh module of Salome with NetGen (there are couple of NetGens, we need particular one). I used additional hypothesis in "3D" tab to introduce layers and played with them to obtain required Y+ (less than 1.0) but also to provide enough layers in turbulent part of boundary layer (it's a small case, [300...500]*10^3 cells, so it runs fast on a PC). IMHO, Line Plot in ParaVis (ParaView) of tangential velocity in near-wall region is a good tool for estimation of boundary layer modelling quality (because it's easy to distinguish "linear" and "logarythmic" parts). And, of course, a surface plot of Y+.
SIMPLEC to SIMPLE ... looks like it is the main responsible for the differences
IMHO, it's very strange. SIMPLE, SIMPLEC and PISO are velocity-pressure coupling methods and, as far as I know, they has nothing to deal with so large differencies of results (if we have a converged solutions). I hope I will check this on my test case.
I still need a very long time (about 16 hours) to finish the simulation
Please check the number of "linear" iterations (tables with rows starting with "c"). If you see more then 100 "linear" iterations for velocity then there may be a problem with mesh or timestep (if SIMPLEC is used). Would you please tell me what is the time per iteration (from Saturne's output) and how many cells your current mesh consist of?
I perform tests on a usual PC (4 x 2600K cores) and it takes just about 30 minutes to obtain several hundrerds of iterations on ~500'000 cells mesh (Saturne 4.0.0).
Yvan Fournier
What may be the reason for this big difference between SIMPLE and SIMPLEC? I can't get how does it possible for coupling sceme to affect the results in such extent... I'm interested in pressure drop calculations too so it's important to me.
There should be no significant difference between the different SIMPLE, SIMPLEC and PISO algorithms, but there might be a slight sensitivity of the results to the time step du to the Rhie and Chow coupling (a disadvantage of colocated discretizations). Still, as the time step is local for steady methods, this is surprising, and the difference should be very minor.
Did you check the Courant/CFL values in the "listing" are close to 1 ? If not, the minimum or maximum time step value might be off.
Also, although it is important to converge computations for more precise results, the pressure drop itself usually varies only slightly, as it is often due mostly to the potential flow (established after the first iteration), then, often to a lesser degree, to the velocity and turbulence characteristics.
So it would be interesting to see how the pressure drop evolves over several iterations :
- if it does not evolve much, you can run comparison tests with only a few iterations
- if it evolves much, this would tend to indicate the turbulence model, or its parameters, are the major factor explaining the difference.
So in any case, checking this evolution of 20 or less time steps (and comparing to the results you have with many more iterations) can provide useful information.
I performed some simple tests yesterday. It was my test case with irregular inlet velocity profile: http://code-saturne.org/forum/viewtopic ... 8934#p8934 http://code-saturne.org/forum/download/ ... &mode=view
Pure aerodynamic, air, without head loss, isothermal, Steady. There was two setups:
1. SIMPLEC, defaults + reference time step 0.01 s.
2. SIMPLE, defaults.
Every case was allowed to calculate ~300 iterations. Then I compared pressure profiles in the slice just after inlet with ParaVis (ParaView) and found no sufficient difference. But there was no any large pressure difference (air) and flow pattern is different from valve. I plan to compose a dummy geometry more resembling the valve and repeat tests (if the reason will not be foubd here at that moment).
Update
====
Sorry, but I had no success with "valve test". I still have Saturne only on my home PC (where there is no SolidWorks) and I can't import "abstract valve" geometry in Salome (some bug in STEP reader). I did another calculation (for my work) on swirling nozzle geometry and calculated pressure drop was consistent (~20%) with simple formula (0.5*Rho*w^2). Settings was Steady + SIMPLE, Upwind for velocity, without flow reconstruction. Now I need to set exact initial data, perform more iterations and "precision run" with Centered scheme for velocity + flow reconstruction, but I don't think that resulting pressure drop will differ significantly from simple estimation.
However nozzle case has geometry far different from valve, therefore I will now take an Internet survey on Salome STEP import bug...
Update 2
======
Hello. I worked with abstract valve geometry yesterday night. A saved this geometry in SolidWorks as STEP and played with STEP version, meters/millimeters and changing geometry. It didn't help. Looks like a bug in Salome geometry import (though two other previous geometries imported correctly). So I used IGES + create shell + create solid, but I only had a time to build the mesh, then I switched to other case (needed to calculate a pressure drop on nozzle for my work). Hope I will get the valve test results soon (SIMPLE vs SIMPLEC).
Hallo,
sorry for the delay. I had a look at the listing files and saw that Courant number is way off (greater than 1 for SIMPLEC simulations).
So the next step will be to play with time step.
Are there any good practices to set minimal/maximal time step factor and maximal variation or should I just play with time step and let the defaults?
The number of linear iterations is much greater than 100 in each test.
I also tried to mesh as Antech suggested, but I'm finding difficulties, as the mesh is fairly complicated.
I think I'll try to make some experience with a simpler geometry.
Ccaccia73 Courant number is way off (greater than 1)
AFAIK, for Saturne it may be up to 20 (50) without problems, although 1...5 is recommended.
The number of linear iterations is much greater than 100 in each test
Maybe it's reasonable to switch to BiGCStab linear solver and set tolerance 10^-5 for all variables (even if you'll reduce the time step). IMHO, it will not affect precision.
Sorry, cannot help you with mesh because your geometry is confidential (and my test case is on my home PC). But I foud it relatively simple to introduce prism layers provided you have marked groups (surfaces).
Ccaccia73 In my case there are small regions where Courant number is > 100
May be it's a reason to use SIMPLEC with local timesteps. They are local spatially in Saturne, AFAIK.
I created a topic on Salome forum, there is an attach with "abstract" geometry outline. http://www.salome-platform.org/forum/forum_10/439129971
Geometry internals shown in attach to this message. Is this kind of geometry relevant? (I'm not working with valves, we use valves from another companies.)
Ccaccia73
Thanks for geometry. I see that it's not a "classic" valve, looks more like a hydraulic switch, if I got it right... I understand that particular details are confidential so I will work with my "classic" abstract geometry. Hope that conclusion about SIMPLE/SIMPLEC sensitivity will be applicable also to your tasks.