CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Transonic rotor convergence problem (http://www.cfd-online.com/Forums/cfx/24168-transonic-rotor-convergence-problem.html)

Abdus Samad June 22, 2007 09:10

Transonic rotor convergence problem
 
Friends,

I am trying to simulate transonic axial compressor using CFX11. I generated fine mesh(300,000 nodes approx.) using Turbogrid and I kept boundry nodes such a way that it will produce y+<1 (I checked it from CFX post).

I tried to run the compressor in design flow rate setting physical time step=1e-5.RMS=1e-5.

But problem is coming in convergence. I changed timestep as per tips given in CFX user guide,but below 1e-5, it is showing sinusoidal residial. If I use time step=1e-5, till 100 iteration it sows good convergence and after that it starts sinusoidal nature.

Using all efforts, I got output mass flow below or less than design flow rate. The efficiency and pressure ratio is coming less than the experimental one. I am checking it from axial compressor report template.

I tried lots of times,if any one has experience of simulating rotor37, please help me to sort out the problem.

Thanks in advance.

Glenn Horrocks June 24, 2007 21:44

Re: Transonic rotor convergence problem
 
Hi,

Have you gone though the documentation "Tips on obtaining convergence"? Also have a look at the best practices guide, also in the doco.

Glenn Horrocks

Abdus Samad June 24, 2007 23:38

Re: Transonic rotor convergence problem
 
Dear Horrocks,

I have gone through the tips and best practice guide. Those says the time step should be within 0.1/w to 1/w.

I went through all the posts in this forum related to convergence problem. Some says initially keep time step little small and bump up by 5 or 10. started time step =1e-5 and if i bump up by 10 ie if i make time step=1e-4 after 10 or 20 step, after sometime it stops showing error and residual window shows very high Mach number.Sometime the regular pattern(sinusoidal) starts with some specific timestep instead of going down to reach the target RMS.

I cheked the mass flow, if I set it design flow (20.19 kg/s), the compressorRotorReport shows mass flow is different than design flow. As a result the pressure, efficiency and other parameters are different from the expected value (high different from the values calculated using CFX by the other researchers).

How much imbalances is acceptable?is it hard 0% or any other value is acceptable?

What should I do? Please suggest.

Pankaj June 26, 2007 05:43

Re: Transonic rotor convergence problem
 
Hi!

I think 1/w is more than enough as your physical timescale.

Use mass flow specified outlet and total pressure and temp (which are the stagnation conditions)at inlet.

Refer tutorial of Centrifugal compressor(new in cfx-11)for more ideas.

Your Imbalances should be less than 0.1%.

There are many other factors need to be considered but it depends on how u have defined the physics and also on your geometry and mesh.

Samad June 29, 2007 10:36

Re: Transonic rotor convergence problem
 
Thanks Pankaj.I will try and I will be back if I face problem again.

KBanks July 4, 2007 04:21

Re: Transonic rotor convergence problem
 
For a transonic rotor, it is often better to start with a static pressure outlet, instead of a massflow. Indeed, in many cases, you will never get a massflow outlet to converge.

Try setting the static pressure at outlet to be much lower than it actually is in reality to help get the case "started". You can then steadily increase the pressure up to the design value using "Edit Run in Progress" in Solver Manager. If you wish, you can then use these results as you initial guess for a run with a massflow outlet. Depending on the case, it can also be helpful to ramp up the rotational speed gradually.

I would also point out that 300,000 cells is not a "fine" grid for a case like rotor 37. If you want a y+ of 1 and a grid fine enough to resolve any shock, you'd require a grid closer to a million nodes. That's not to say 300,000 isn't useful, it just depends what you are interested in.

Hope this makes sense,

Regards,

Kevin

metaliat93 February 16, 2016 14:13

2 Attachment(s)
[QUOTE=KBanks
;82442]For a transonic rotor, it is often better to start with a static pressure outlet, instead of a massflow. Indeed, in many cases, you will never get a massflow outlet to converge.
I have some problem with parametrs
Attachment 45227
Attachment 45228

turbo February 16, 2016 17:18

Do not use the mass flow rate at the exit BC in compressible flow CFD. Originally the option was not available in any of CFD in turbomachinery area. It was born by many requests from users for convenience to get the target flow rate in a single shot. In physics, it will induce instability in convergence. Use (Po, To, flow angle) at inlet always, and Ps at the exit always. PLEASE !

turbo February 16, 2016 17:21

Fine grid is not always better in convergence due to the relative error magnitudes. Try to reduce the mesh size a little bit and use automatic time scale (that is good enough).

Opaque February 16, 2016 17:48

May I ask what version of the software you are running ?

If you are running version R15, or R16, and you have a good idea of the corrected mass flow through the machine, you may want to give a try to a newer mass flow boundary condition developed for ANSYS CFX, named "Exit Corrected Mass Flow".

Unlike the classic exit mass flow condition which has fairly robust convergence between stall and away from choke, the newer option is fairly robust across the whole range of the machine from stall to choke w/o you having to change the outlet boundary condition.

Summary: you should be able simulate the complete speed line (performance curve) by just changing the amount of mass flow in the range of interest.

Hope the above helps, and good luck

metaliat93 February 17, 2016 06:43

Quote:

Originally Posted by turbo (Post 585555)
Fine grid is not always better in convergence due to the relative error magnitudes. Try to reduce the mesh size a little bit and use automatic time scale (that is good enough).

I used static pressure in the outlet, and total pressure in the inlet.
I check different mesh. On graff results on mesh 500 000 elements.

metaliat93 February 17, 2016 06:43

Quote:

Originally Posted by Opaque (Post 585561)
May I ask what version of the software you are running ?

If you are running version R15, or R16, and you have a good idea of the corrected mass flow through the machine, you may want to give a try to a newer mass flow boundary condition developed for ANSYS CFX, named "Exit Corrected Mass Flow".

Unlike the classic exit mass flow condition which has fairly robust convergence between stall and away from choke, the newer option is fairly robust across the whole range of the machine from stall to choke w/o you having to change the outlet boundary condition.

Summary: you should be able simulate the complete speed line (performance curve) by just changing the amount of mass flow in the range of interest.

Hope the above helps, and good luck

I use version 16.1 ansys CFX


All times are GMT -4. The time now is 12:31.