CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   When to use local timescale or physical timescale (http://www.cfd-online.com/Forums/cfx/85612-when-use-local-timescale-physical-timescale.html)

 xyq102296 March 2, 2011 11:31

When to use local timescale or physical timescale

I am using ANSYS12.1 to simulate, but recently I met a problem
after mesh and adding all the boundary conditions, I use physical timescale t=2s to simulate
while now I use local timescale factor and use default value 5 to simulate, the result distributions turns out to be slightly different, so which timescale shall i use?
I am really confused now

 ghorrocks March 2, 2011 17:39

This FAQ explains timescale selection and when to use local timescale factor:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

 xyq102296 March 3, 2011 05:28

Quote:
 Originally Posted by ghorrocks (Post 297696) This FAQ explains timescale selection and when to use local timescale factor: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
Ghorrocks, firstly thank you very much!
before I asked this question, i have already searched the FAQ, still I have the problem.
From the text, he uses "Use a larger physical time step" first, and then Use Local Timescale Factor? So when I trying to solve my simulation, which option shall I use? and what's the time scale is appropiate to use? 1s? 5s? or 10s?
in my simulation, both can converge under 10e-5, but the temp and velocity distribution is slightly different

 ghorrocks March 3, 2011 18:46

This is all discussed in the page I linked to.

 xyq102296 March 4, 2011 04:21

Quote:
 Originally Posted by ghorrocks (Post 297854) This is all discussed in the page I linked to.
Use a larger physical time step. A time step approximately equal to the average residence time in the simulation domain is a good guide for most simulations. If it is a recirculating system without an inlet or outlet then use the turn over time of the largest flow feature. You can get the residence time in CFX-Post by placing a streamline and looking at the "Time" variable on it. The maximum value of time is the residence time.
Use Local Timescale Factor. A factor of about 5 is a good guess to start with. If this is successful you should run the final few iterations to convergence with a physical timescale (not local timescale all the way to convergence).

That's all i seen from that page about timescale, it doesn't describe which to choose and what's the appropriate number.........

 ghorrocks March 6, 2011 18:07

The FAQ is written as a step by step guide as how to address the non-convergence. It discusses adjusting the timestep later on:

Quote:
 Do a test run with the residuals included in the result file. It is likely a small region of the flow has high residuals while the rest is converging. Consider why are the residuals high in that region - Is it: Poor quality mesh - the fix is obviously do a better quality mesh A physical instability, such as vortex shedding - the fix here is to use a larger timescale, a coarser mesh in the vortex shedding region, decrease the blend factor (if using hybrid differencing) or use a lower order turbulence model. The first option is preferred as the latter options can have accuracy implications.

 xyq102296 March 7, 2011 05:58

but here, if I try to use physical timescale,
from the link you gave me, "A time step approximately equal to the average residence time in the simulation domain is a good guide for most simulations" I checked my result file, min=0s and max=84s, so average is 42s?
WHile from the CFX help file, "time scale should be not larger than the advection time scale value" in order to get convergence which is only 2.75s

so which number shall i choose, and what's the real meaning behind the number?

 Attesz March 7, 2011 08:17

I've tested the timescale problems recently. In my multidomain heat transfer (solid and fluid) simulation I've used automatic timescale first with conservative, then with aggressive by adjustin the factor from 1 to 10 step by step to avoid divergence. Because of the time need of the convergence in case of complex heat transfer (with heat source) problem, this can help to shorten convergence type. But if you choose large timesteps (large timescale factors or physical timescale doesn't matter) the residuals remains "high". After in my simulation the imbalances were under 0.1, a swithed to physical timescale with very small value. So the RMS and also MAX values decreased fast, as the imbalances do.

 ghorrocks March 7, 2011 19:45

"time scale should be not larger than the advection time scale value" - where did you see that? I cannot find this comment, and it is incorrect in my opinion. The time scale SHOULD be larger than the advection time scale for a steady state simulation to reduce flow vortex instabilities.

 xyq102296 March 10, 2011 03:58

Hi, Ghorrocks

I tried large physical timescale under High Resolution Advection Scheme, and my imbalance is under 0.02%, RMS value reached the 1e-06. Does this mean my simulation is correct and converge?

WHile from the help file "Problem with Convergence" : if the MAX residual is more than one order of magnitude larger than your RMS residual, it usually indicates that the problem is concentrated to a local region.
and I found two of " Locations of Maximum Residuals " is close to my interested region, does this matter?

 ghorrocks March 10, 2011 07:25

Quote:
 Does this mean my simulation is correct and converge?
Converged - almost certainly, but you should do a sensitivity check to be sure. You are probably converging tighter than you need.
Correct - Cannot say. There are many checks you need to do beyond just convergence to get a correct solution. And no, I am not going to write them all up on the forum, I will refer you to CFD text books for that. Computational Fluid Dynamics by Roache is one of the key textbooks for CFD accuracy.

 xyq102296 March 10, 2011 08:41

Hi

While from the help file "Problem with Convergence" : if the MAX residual is more than one order of magnitude larger than your RMS residual, it usually indicates that the problem is concentrated to a local region.

In my simulation, MAX residual is more than one order of magnitude larger than RMS residual, and two out of four " Locations of Maximum Residuals " is close to my interested region, so do you know any methods to decrease the value difference to eliminate the influence?

 ghorrocks March 10, 2011 20:24

Improving mesh quality is usually the biggest difference.

 xyq102296 March 21, 2011 09:18

Hello, Ghorrocks,

I tried to modify the geometrical mesh quality a bit and rerun the program. THe result didn't change much......

Here I used both High Resolution and Specified Blend Factor=1 methods and set the RMS residual=1e-05, will the result be very similiar accroding to the theory? Becasue both are second-order accurate.

 xyq102296 March 21, 2011 10:18

Another question, if I use Specified Blend Factor=1 here, what will Local time scale and Physical time scale make any difference in simulation?
From ANSYS help file,
Local Timescale Factor allows different time scales to be used. It's best for uniform element and moderate aspect ratio.The default value is 5, what's the meaning of 5 here?
Physical Timescale allows a fixed time scale.
My model has great aspect ratios and with non-uniform elements, so which option is best for my model? Because my simulation is under steady situation, will these two timescales matter much?

Too many questions , heihei, Thank you in advance!

 ghorrocks March 21, 2011 20:10

Quote:
 will Local time scale and Physical time scale make any difference
Yes.

Local time scale really only needs to be used for difficult problems. Most problems should be OK with physical time scale.

 xyq102296 March 22, 2011 02:10

But here if I use physical timescale and set RMS residual =1e-06, it takes me 24hours to converge, while if I use local time scale and use default value=5, it took me one day to reach 1e-04 rms residual, and I checked the CFD post, the shape of distribution is different from Physical timescale. 1e-04 is just for demonstrate the basic shape and i am not sure how many days will it take to reach 1e-06.....so I wonder is there a way to speed up the converge

 ghorrocks March 22, 2011 07:48

The CFX documentation describes how to speed things up. This link may also be of assistance.
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

And of course you can always stick more computers on a parallel network to speed things up.

 mejahan August 7, 2013 14:36

Can you please tell me how I can check the regions of max residuals ,

Thank you.

 ghorrocks August 7, 2013 18:31

When you set the simulation up, in the CFX-Pre output tab add the equation residuals to the results file. Then the residuals will be part of the output file and you can use standard post-processing techniques on them as a normal variable.

All times are GMT -4. The time now is 11:54.