CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

problems by changing turbulence modell

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 8, 2015, 04:54
Default problems by changing turbulence modell
  #1
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
Hello again,

I have some problem by changing the turbulence modell from k-epsilon to k-omega-SST.

When I use the k-epsilon modell I get a steady state solution for my problem. Now I have to change the turbulence modell to k-omega-SST and when I use "advection scheme: upwind" and "turbulence numerics: first order" i get a converged steady state solution, too.
But I read, that for final results I should use the "high resolution" option for both.
When I use the high resolution option my residuals will decrease within the first 100 timesteps, but then they increase to the value 1e-3 and the values on my monitor points are oscilating.

Can I use the first order and upwind option ?
Do someone know the problem and a solution for it ?
biro is offline   Reply With Quote

Old   January 8, 2015, 05:13
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Not all simulations are sensitive to tight convergence of the turbulence equations. I would do a sensitivity study to see if it makes a difference in your case. Loose convergence of the turbulence equations may be irrelevant, making it unnecessary to converge tighter.

Also this FAQ may help:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   January 8, 2015, 06:05
Default
  #3
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
I read the FAQ, but I don't find an item, which can help me.

Can you give me a short explain, what kind of sensitive study you mean ? I don't know this time what you mean.



Maybe my explanation are not exacty: all my residuals increases, not only the residuals for turbulence
biro is offline   Reply With Quote

Old   January 8, 2015, 06:34
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The big tip on the FAQ is try a bigger time step. Have you done this? Also improved mesh quality ALWAYS helps.

Sensitivity study: Do a simulation at one convergence value (1e-2 maybe) and another to a significantly tighter value (say 1e-3) and compare the results for a value of interest to you. If it has not changed significantly then it you can be confident you are OK and can stop there. If it has changed then you need to try tighter again (1e-4) and keep going until it converges.

If you can't do this using high order turbulence (you might not get tight enough convergence) then it should be OK to do the sensitivity study on low order turbulence and use that result for the required settings for the high order turbulence simulation.
ghorrocks is offline   Reply With Quote

Old   January 8, 2015, 14:53
Default
  #5
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
Sorry for my answer there was no item in the FAQ! I wasn't concentrate enough, but my time is runing out for thesis. And slowly I get panic


I have varied the timestep size from residence time (rt) over rt/2, rt/3 to rt/4.
You will see, that the convergence is even better and the monitor point iss steady state. But the convergence of the turbulence rms is still bad.

In the last picture you will see a stagnation region after a tear-off edge. I need the tear-off edge to slow down the stream to reach the velocity profile I need. I think, that the stagnation region is responsible for bad convergence ?! But with the k-epsilon model there was no problem ?! And I use the same mesh (y+ = 50-80). I thougt (with automatic wallfunction) the solution has to be similiar with both models.

My plan was to change turbulence modell (with same mesh as k-epsilon) and then to refine to y+ ~1


One more question: your said "... then it should be OK to do the sensitivity study on low order turbulence and use that result for the required settings for the high order turbulence simulation."
Which settings do you mean ?
Attached Images
File Type: jpg rms_residence_sst_001.jpg (53.2 KB, 10 views)
File Type: jpg rms_turb_residence_sst001.jpg (47.8 KB, 11 views)
File Type: jpg ReInlet_residence.jpg (38.9 KB, 9 views)
File Type: png streamlines.png (19.3 KB, 11 views)
biro is offline   Reply With Quote

Old   January 8, 2015, 16:42
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Also try time step size larger than the residence time.

If you do the sensitivity study I suggested using low order turbulence (so you get tight convergence) then you can use those settings on the high order turbulence simulation. It might be tricky to get the high order turbulence to converge tighter so it is best to know if you need to before you do it.
ghorrocks is offline   Reply With Quote

Old   January 10, 2015, 06:22
Default
  #7
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
By using timestep larger residence time I became worse convergence than I use rt/4.

I have problems by doing the sensitivity study:
When I use convergence criteria 1e-2 or 1e-3 the criterias are reached after the first respectively after the second iteration. But my values of interests can't adjust within 2 iterations.
What can I do ?
biro is offline   Reply With Quote

Old   January 10, 2015, 14:46
Default
  #8
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,188
Rep Power: 23
evcelica is on a distinguished road
You clearly have transient flow, so It is very difficult to converge the numerical residuals using a steady state solver. But that doesn't mean that you don't have a good solution, if your result of interest isn't changing then you should be good. I'd concentrate on sensitivity analyses and grid refinement and check to see if your result of interest isn't changing. Don't worry about the value of the residuals.
evcelica is offline   Reply With Quote

Old   January 10, 2015, 15:15
Default problems by changing turbulence modell
  #9
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
Thank you for your answer evcelica.

I will do refine-mesh-study and show on the value of interest.
But I don't know how to do a sensitivity analysis, can you give me a short explanation how to do?
biro is offline   Reply With Quote

Old   January 12, 2015, 17:18
Default
  #10
Member
 
Robert Bischof
Join Date: Aug 2014
Posts: 56
Rep Power: 12
biro is on a distinguished road
I try to execute a transient simulation. After 40 timesteps everything went well and every variable has a good value.

But the adaptive timestep algorithm falls back to a timestep of 6.5e-5 [s] so I think, the timestep iss to small to see anything ?!
And the Courant-Number (RMS) has a value of 131.5 (max Courant Number 999.99). I thougt Courant Number should have be a value of about 1.

So I think I simulate a kind of rubbish ?! Can everybody help me ?
biro is offline   Reply With Quote

Old   January 18, 2015, 06:47
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Use adaptive time steps homing in on 3-5 coeff loops per iterations. Do not use Courant number adaptive and ignore the Courant number reported. It is not relevant for many flows.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Viscositymodel tutorial, problems when changing test case to cavity sur4j OpenFOAM Programming & Development 1 December 8, 2013 10:53
[ICEM] Problems on changing geometry inside a domain andrew12321 ANSYS Meshing & Geometry 4 November 18, 2013 18:36
specify the turbulence intensity and the turbulence length bennoman75 Main CFD Forum 0 May 15, 2013 06:36
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 21:28
Turbulence boundary values lego Main CFD Forum 0 October 24, 2002 14:47


All times are GMT -4. The time now is 04:37.