Hi!

I am having a little problem with convergence. I am trying to simulate flow through orfice plates, but i cant get cfx to converge. I tried to change physical timestep, but no succes. I altered the mesh by reducing the number of nodes and it converged, then I used this solution for initial values and still nothing. The convergence criteria is 5*10^-4. Equations are 2nd order. If equtions are 1st oreder it converges, but results I get are not what I hoped for. In fact I am trying calculate coefficients for different diameters of orifice plates, but they seem to be quite random. Is there anything else to do?

And another thing: I tried to use symmetry planes but this eksperiment gave totaly different results then the one with the hole domain. Why is that?

Thx for help!

Beno

I am not sure if I can help you, but I am very interested if/when you get some results . (I only use 5.5.1, so if you are using 4.4 this is not a help and if you are using 5.6 it might be valid. Please in future specify version) Here a a few points that has helped me in the past.

How much did you change the physical time step? I assume you mean the "pseudo" time step for the calculations in the solver options or are you calculating transient? Try to use one, based on length and speed parameters for your application, maybe orifice velocity and diameter, a factor of say ten of this time? You could also try to look in the out file for advection time, then try to use say (again), this time divided by 10. This approach seems to help me when using 2nd order. But try to look at the "time" in the orifice, that is at least a physical time.

You could also be having some problems with controlling you mesh, you don't mention much about it. It could be worth to use some mesh control parameter at the location of your orifice plate. Maybe a line through the holes where you specify the lenght scale. A reason for the difference with the symmetry planes could also be, (depsite a possible problem in CFX, which ) if you are having too large differences in the grid, the mesh control will help you deal with this.

Have you used inflated boundaries at the walls? they can give problems, but you should use them.

Is it all diameters that cause problems, what range of porosity are you investigating? I am thinking about if you calculate very small porosities then you will locally get a huge acceleration of the flow. I do not know if that is a specific problem with the solver, but I could imagine that it could lead to problems. Again in this case, the control of the time step could help.

A wild guess, have you checked your Mach number in the orifice? compressibility problems - probably only for very small porosities.

Hope I could be of any help and if possible please inform me when you get some results if you are willing to share them.

Regards Jan

Hi Beno and Jan,

Jan has some good comments, but I will add a few other things to check. Check the following:

1) That the simulation is physically possible (not exceeding choked mass flow rate if compressible etc) 2) Try running the simulation with upwinding differencing first, and using that as an initial condition for the final run to accurate convergence using a second order scheme. 3) Check your mesh is OK. Check y+ is OK at the walls, elements are not too large or distorted, and adjacent elements are not too different in size (Try to make the volume of any two adjacent elements different by at most 20%. For highly grid sensitive regions, eg seperations, you need to make this more like 5% or less) 4) Try smaller timesteps. If you already are using very small timesteps, try larger ones. If you have are using a turbulence model and your timestep is of the same order of the turbulence time scales then convergence can be poor 5) If after all that you still can't get it to converge as a steady state simulation, then there is probably no steady state solution due to some form of vertex shedding. You will have to run the simulation as transient.

Please note that these comments are pretty much the same comments that we give anybody who can't get convergence. If you are having problem with convergence in any type of simulation the above points are things to check. Also refer to the CFX manuals, they have quite a good introductory discussion on methods of getting convergence.

Regards, Glenn Horrocks

Hi' Glenn, Excellent comments, but I disagree on one point. I really can't be neccesary with transient calculations for this kind of problem, then the problems is elsewhere the code or grid or setting up the problem, etc.

Hi Jan, why do you say that (not disagreeing with you, just would like more explanation)?

I read in the Menter AIAA paper on drag prediction that there was a separation bubble that caused problems (engin pylon if I recall - can't remember the solution). Would this be the same sort of problem that Beno could be experiencing and that Glenn was refering to ? Or would that not be an issue off a sharpe edged separation ?

I agree that all of the other suggestions should take a higher priority before moving the transient effect being the cause of the problem.

Bob

Hi' Bob

I have not read the Menter paper, but it sounds interesting I will have to get it, thanks. But I have and many other people have succeded on doing steady state calculation of orifices and that was the only reason for why I stated it should not be neccesary with a transient calculation. (sorry not very scientific, just experience) I know that solving a problem transient can help convergence problems, but I think in many cases that the convergence problem could have been solved in other ways (well not for true transient problems )

Have your checked the paper on the community pages: FLOW IN PIPES WITH SUDDEN CONTRACTIONS: CFX-5 PREDICTIONS AGAINST EXPERIMENTAL DATA Authors: Francesca Iudicello Reference: ANSYS CFX, UK User Conference 12th November 2003, Coventry, UK It is only one orifice, but there could be some hints.

Hi,

In my experience, the majority of real-world simulations involve some sort of transient feature, even if the boundary conditions are steady state. Somewhere in the model there is always a bit which is shedding vorticies. (Maybe this is just because I always do simulations in this flow domain?)

A simulation which is almost all steady state, except a small bit with transient shedding usually manifests itself (in a steady state simulation, with all other parameters correctly set) by initially converging well, but the residuals stop and leveling off at some point before the convergence critereon is met.

Usually the only way to get this one to converge to the desired critereon is by changing to a true transient simulation with a fine enough timestep. But depending on what you are trying to do, the original not-quite-converged steady state solution might be OK as some sort of average response.

Regards, Glenn

Hi Glenn,

I agree that almost all fluid problems are in someway transient, well thats the nature of turbulence aswell. I always search for a steady state solution if one exist. For my engineering applications that is sufficient in most cases. I do not have problems with averaging I am therefore also satisfied with RANS codes beecause I think as you wrote "might be OK as some sort of average response". Same trick with turbulence I do not mind RANS codes, the turbulence is time depandant but I guess, that you, based on your post that you always do DNS, LES or whatever then. )) Regards Jan

Hi Jan,

Even with RANS simulations you can still get shedding in certain Reynold snumber ranges. This is what I meant, rather than DNS/LES. DNS/LES is far too hard for my small brain.

Glenn

Hi'

What?? I don't think your got my point, I just thought it was funny that you stated calculations should be done transient, always, to get it as true as possible. I had the impression that you then didn't like averaging. If that is true then your should not use RANS codes ), right !?

Hi Jan,

What I mean is this. In a real flow, there are flow features ranging from the smallest, high frequency turbulent eddies, through to larger turbulent eddies and on to eddies which are of the same scale as the geometry. In DNS you resolve all frequencies. In LES you resolve the larger turbulent frequencies, but use a model to handle the highest turbulent frequencies.

In RANS, it is not so clear. You certainly use the model to handle both the small and large turbulent frequencies, but what about the eddies which are of the same scale as the geometry? In my experience if you use a coarse mesh/timestep you often do not resolve these frequencies, but hopefully its effects is included by the turbulence model. If you use a finer mesh/timestep you often resolve these geometry scale frequencies.

What this means about the steady state or transient thing is that if a RANS simulation does not converge adequately in steady state, then it probably has model scale eddies in it, and to resolve them you need to use a transient simulation. Using a coarser timestep or mesh might also stop them by using the turbulence model to handle the fluctuations and giving you a steady state answer, but this is problem dependant.

If there was a simple answer then CFD would be boring.

Regards, Glenn

Hi Jan / Glenn,

its interesting what you are saying Glenn as I have found similar results. When modelling, 2nd order, i have in the past conducted mesh refinement studies. On refining the mesh I have struggled to achieve convergence. Often the only way to converge on a steady state solution was to set a blend factor of 0.6-0.7. However If my understanding is correct (please correct me if not), setting a lower order differencing scheme has the same effect as coarsening the mesh.

When running the same problem transiently, convergence was achieved. But for how long should I then run this simulation. Transient effects always take a long time to present themselves (eg vortex shedding behind a circular cylinder - takes time to start and then more time to settle). So how long should you leave the simulation ? In the past I have stopped runs, and observed no transient effects, but the convergence was great. Did I stop the run prematurely ?

Wouldn't if be nice if once in a while CFD were simple !!

Bob

Well, I guess I must have been very lucky in the past. I always use the higher order. If I ever had convergence problems it has always been solved by adjusting the grid or changing the "false" timestep or adjusting parameters stepwise etc.. For true non steady state problems I have of course solved them as transient, but my experience really tells my that the problems is elsewhere than switching to transient. But what the .... if it helps - so why not solve it transient, but as you have mentioned some other problems arise.

Hi again (after a time)!

As a matter of fact I have tried most things that you suggested: timesteps, mesh controls, inflated boundary… No succes. Maybe I can do something with the mesh. If I coarse it, the convergence is faster but that also influences results.

There is also an interestin phenomena: the vortex behind the orifice can be unsymmetrical, either it "swings" up or down.

Is it ok if I use monitor points to monitor e.g. velocity, and when it converges to a certain value check for results? I tried to use monitor points but I don't know how to write this results to a file. In manual I only found how to write out results in DOS nad even then I cant help myself with the output..

Now I am trying with a blend factor 0,65, and I will see what I get. I am also doing transient calculation.

Jan, I can send you (email?) results and files, however I am not very experienced in numerics, but I hope it helps you. But as I said, they are not what they are supposed to be.

A friend tried to do the same thing in Fluent and everything but velocitiy converged well.

Anyway, thx for help!

Beno

Another thing: I use v5.5.1.

Beno

Beno Would you mind telling what is the ofirice velocity, free stream velocity, orifice diameter and fluid properties. Jan

Velocity is 0,1 m/s to 10 m/s Diameter of pipe is 200 mm orifice diameter 40 to 150 mm fluid is water at rtp (cfx library) for some cases maximum velocity at the orifice is extreme (337m/s), but for some is ok (0,2 m/s).

Anything else?

Beno

Hi!

http://users.kiss.si/~k4fs0371/

here are some jpg pictures of my problem.

Beno

Hi Beno,

From your pictures of your mesh it is obvious that the mesh is not very good for this type of problem. It depends on exactly what you want to get out of the simulation, but if you want accurate pressure drop versus flow rate simulations you will need to do the following:

1) The mesh in the oriface area is far too coarse to resolve the flow accurately. You will need to reduce the element edge length by at least a factor of 2 and maybe more. Do a mesh independance study to establish the mesh you actually need.

2) The mesh downstream of the oriface is too coarse also. Need more elements here too.

3) The prism layers are making a poor quality mesh in the oriface region. I would use less prism layers, but this problem may be eliminated when you improve the mesh density as suggested in 1 and 2.

4) Is the flow is from left to right? Is the flow fully developed when it reaches the inlet? You may be able to shorten the left hand side if you can impose the fully developed profile at the inlet (maybe down to 5 diameters, or even less).

5) You will also need to model further downstream for the high Reynolds number simulations. Start at about 10 pipe diameters downstream, and keep increasing until it converges nicely and the pressure drops don't change between different downstream lengths.

Hope this helps, Glenn