[Tingyun YIN]

Hi everyone.

Currently I am working on the compressible flow with CFX. Following up the CFX HELP DOCUMENT, a unsteady calculation was established. But I got some problems during running. After checking some previous thread, no relevant suggestions were found. So, I come here for help.

As shown in Fig, 20 iterations were calculated within each time step, though RMS has already dropped below 10-4, which confused me a lot. It should be noted that the incompressible calculation ran successfully. Also, mesh was much refined, Y+ is around 1. Total energy was turned on. SST model was employed. Fluid density is the function of pressure. A reasonable initial result was obtained with steady compressible flow. Besides, adaptive time step was tried but failed.

Any comments will be appreciated. Thanks in advance.

[Opaque]

H-Energy has not converged yet.

[Tingyun YIN]

Originally Posted by Opaque

H-Energy has not converged yet.

Thanks for your reply.

Now that H-Energy is still higher than 10-4, are there any effective methods to drop it?

[Opaque]

Do not stop the run, let it converge until it reaches the appropriate residuals.

There are guidelines to improve convergence in the documentation.

[Tingyun YIN]

Originally Posted by Opaque

Do not stop the run, let it converge until it reaches the appropriate residuals.

There are guidelines to improve convergence in the documentation.

See. That's also the reason why compressible has more convergence problems than incompressible flow..

[Opaque]

In your case, what is your setting for the Maximum Number of Coefficient Loops ? I can only guess it is 20, increase it and see if the energy equation converges.

I can also see from you diagnostic output you are solving a transient homogeneous multiphase compressible flow. There may be all kind of non-linearities and w/o understanding the details of the physics you are modeling and there is no one answer that makes all compressible flow to converge.

[Tingyun YIN]

Originally Posted by Opaque

In your case, what is your setting for the Maximum Number of Coefficient Loops ? I can only guess it is 20, increase it and see if the energy equation converges.

I can also see from you diagnostic output you are solving a transient homogeneous multiphase compressible flow. There may be all kind of non-linearities and w/o understanding the details of the physics you are modeling and there is no one answer that makes all compressible flow to converge.

Yes, you are right. For my case, cavitation is simulated with homo-mutiph-compre-transient method. Following your suggestions, maximum number of coefficient loops are increased till 100, convergence problem of H-Energy still can not be avoided, which is a big problem.

[Gert-Jan]

It is a bit weird that all equations are converged, except Energy. Given the rate of 1.00, I don't expect that even 100 coefficient loops will have any effect. Looks like it is stalled. First advice would be: decrease the timestep. Usually that is more efficient than more coefficient loops.

To nail down the problem you have to look deeper. A few suggestions:
1) What you could do is write out the residuals (Pre>Output Control>Output Equation Residuals) and look in Post where the residuals are high. It can be that it is just a single element that screws up the convergence. Then don't mind, as long as it is in a region that is less relevant.

2) There are 2 options to write out the residuals and monitoring data: 1) the values only at the end of the timestep (=default) but also 2) each iteration within the timestep (Pre>Output Control>Monitor>Monitor Coefficient Loop Convergence). Did you try this? This gives you graphical information on how the convergence evolves within the timestep. This can give more insight, sometimes. Given the rate of 1.00, Energy will be a flatliner I guess. Can you confirm?

3) This option also allows you to monitor the evolution of temperatures (and u,v,w,p,tke,ted, and massfracs) in multiple monitoring points. What do these tell you? Do you see flatliners for T after 5 coefficient loops? Then your solution is not so bad, provided the monitoring points are in a critical region.

If you are lucky, you have placed one of your monitoring point at a position where Energy does not converges very well. Then you might see the temperature is changing continuously (flip-flop). Then, again I would advise to decrease the timestep. Usually that is more efficient than more coefficient loops.

5) Do you monitor mass and energy balances? Do they tell you anything? Is energy far of zero?

6) Other options to investigate are:
- perform a calculation where you not only couple u,v,w&p but also the massfractions.
- use expert parameter volfrc sumapp
The latter two have effect on the calculation of the massfraction, which might help.

7) Don't bother about the residuals. Maybe it is only a problem in the first 10 timesteps.

[Tingyun YIN]

Originally Posted by Gert-Jan

It is a bit weird that all equations are converged, except Energy. Given the rate of 1.00, I don't expect that even 100 coefficient loops will have any effect. Looks like it is stalled. First advice would be: decrease the timestep. Usually that is more efficient than more coefficient loops.

To nail down the problem you have to look deeper. A few suggestions:
1) What you could do is write out the residuals (Pre>Output Control>Output Equation Residuals) and look in Post where the residuals are high. It can be that it is just a single element that screws up the convergence. Then don't mind, as long as it is in a region that is less relevant.

2) There are 2 options to write out the residuals and monitoring data: 1) the values only at the end of the timestep (=default) but also 2) each iteration within the timestep (Pre>Output Control>Monitor>Monitor Coefficient Loop Convergence). Did you try this? This gives you graphical information on how the convergence evolves within the timestep. This can give more insight, sometimes. Given the rate of 1.00, Energy will be a flatliner I guess. Can you confirm?

3) This option also allows you to monitor the evolution of temperatures (and u,v,w,p,tke,ted, and massfracs) in multiple monitoring points. What do these tell you? Do you see flatliners for T after 5 coefficient loops? Then your solution is not so bad, provided the monitoring points are in a critical region.

If you are lucky, you have placed one of your monitoring point at a position where Energy does not converges very well. Then you might see the temperature is changing continuously (flip-flop). Then, again I would advise to decrease the timestep. Usually that is more efficient than more coefficient loops.

5) Do you monitor mass and energy balances? Do they tell you anything? Is energy far of zero?

6) Other options to investigate are:
- perform a calculation where you not only couple u,v,w&p but also the massfractions.
- use expert parameter volfrc sumapp
The latter two have effect on the calculation of the massfraction, which might help.

7) Don't bother about the residuals. Maybe it is only a problem in the first 10 timesteps.

Thanks a lot.

Follow your suggestions, residual and monitors were set to check the calculation. Something different were found. As shown in Fig, Imbalance of Fluid 1 is quite strange, which seems to be the main problem. It should be noted that Fluid 1 is water, of which density is the function of pressure and other properties are constant.

[Tingyun YIN]

Here are residual results.

[Gert-Jan]

The flip-fliop of the energy balance might be based on inaccuracy of the energy equation. Suggestion: Go to double precision. Enthalpy has quite large numbers . Then small variations might be missed in the accuracy.

The imbalances are calculated based on what comes in your domain (I think). If this flow is small, flip-flip behaviour might also occur. So, further advice is difficult to give without knowing your case.

Do you use the built-in cavitation model? Do you really need total energy? Are you studying the thermal effects around collapse of cavitation bubbles?

[Tingyun YIN]

Originally Posted by Gert-Jan

The flip-fliop of the energy balance might be based on inaccuracy of the energy equation. Suggestion: Go to double precision. Enthalpy has quite large numbers . Then small variations might be missed in the accuracy.

The imbalances are calculated based on what comes in your domain (I think). If this flow is small, flip-flip behaviour might also occur. So, further advice is difficult to give without knowing your case.

Do you used the built-in cavitation model? Do you really need total energy? Are you studying the thermal effects around collapse of cavitation bubbles?

Yes! The default cav model was used.

I going to capture the shock wave due to the bubble collapse. Therefore, compressibility has to be calculated.

Fluid 2 is vapor, and Ideal Gas Law was employed. Actually, I am thinking Isothermal Compressibility might also be suitable for current work?

[Gert-Jan]

This is a very difficult task. I doubt if the built in cavitation model is capable of this. CFX uses the simplified Rayleigh-Plesset model. It omitts the second order terms.......
You also need to include surface tension effedcts, which required a superb mesh. Are you aware of these implications?

[Tingyun YIN]

It's different.

Not the abrupt shock wave, it is just the condensation shock, which is the mechanism responsible for cavity shedding.