|
[Sponsors] |
![]() |
![]() |
#1 |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
H-Energy has not converged yet.
|
|
![]() |
![]() |
![]() |
![]() |
#3 |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
Do not stop the run, let it converge until it reaches the appropriate residuals.
There are guidelines to improve convergence in the documentation. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
||
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#9 | |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
Quote:
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. |
||
![]() |
![]() |
![]() |
![]() |
#10 |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
Here are residual results.
|
|
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
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? |
|
![]() |
![]() |
![]() |
![]() |
#12 | |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
Quote:
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? |
||
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
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? |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Member
Tingyun YIN
Join Date: Apr 2017
Posts: 31
Rep Power: 9 ![]() |
It's different.
Not the abrupt shock wave, it is just the condensation shock, which is the mechanism responsible for cavity shedding. |
|
![]() |
![]() |
![]() |
Tags |
compressible flow problem |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Having Problem solving 2D supersonic flow around a plug nozzle | chrislloyd | FLUENT | 7 | July 22, 2015 13:09 |
Problem, adding passive scalar transport for turbulent, compressible flow | cryple | OpenFOAM Programming & Development | 2 | March 25, 2013 11:00 |
Boundary condition for compressible flow ( cavity lid problem) | pike@91 | Main CFD Forum | 2 | June 2, 2012 17:04 |
Negative density problem. compressible flow | Karl | Siemens | 2 | July 10, 2008 16:41 |
Problem on boundry of two phase flow | youngan | CFX | 0 | June 30, 2003 02:32 |