CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Turbulent Boundary condition, viscosity ratio and length scale

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

Like Tree21Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 17, 2012, 03:31
Default
  #21
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
You are right, my Re no is 40.4 times higher. Should I try with a finer mesh so? I'm considering to reduce scale to get a similar case to the one in the reference and compare results. And once then go back to the current scale.
Jonson likes this.
Bollonga is offline   Reply With Quote

Old   October 17, 2012, 03:38
Default
  #22
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
Just reduce your inlet velocity by a factor of 40 and give it a try. If you don't have any problems then, you know that your grid needs some refinement for your current case. (Don't forget to enlarge the timestep, when you reduce the velocity)
RodriguezFatz is offline   Reply With Quote

Old   October 17, 2012, 15:30
Default
  #23
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
Well, Iíve run the case for 0.25 m/s, using the same solver setup and different time steps: 1, 2 and 4 s. Convergence criteria 1e6 as before.
I comment a few things:

1)
Almost no TVR limitation, just a few cells (small vortexs) at some iterations.

2)
Y+ very small, from 0.1 to 1.8. First layer of prism layer should be higher for SWF. (see picture)

3)
Epsilon residuals in some iterations canít go under 1e6.

4) Turbulence intensity drops too fast so close to the inlet. (see picture) Iíve read in the forum that if TI drops too much it means that equilibrium between k and e is wrong because I have too much dissipation, e is over estimated. I guess I need a higher amount of TI in the inlet so I get the desired value at the plate? But if I put too much TI and initialize the solution from the inlet it may start with TVR limitation from the beginning.


5) Lift and drag keep oscillating even if I have left time enough for the flow to run the entire domain for twice (3200s at 0.25 m/s) (see pictures)


Iím gonna try to simulate at the same scale as the reference, with same Re number and try to get a correct y+ value. Once then I'll have to try again the real scale. Any suggestions?


Thanks a lot
Jonson likes this.
Bollonga is offline   Reply With Quote

Old   October 18, 2012, 02:39
Default
  #24
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
Hey,

2) With an y+ of that size: If you can afford that mesh (by means of computational power) you can just use the "enhanced wall treatment" instead of wall functions.
4) I don't know much about that, but what you write sounds reasonable. You say, that TE drops on the way from your inlet to your plate, correct? Now, shouldn't you fix your k and e at the inlet in a way, that the 10% TI is sustained? Or isn't that possible?
5) Your plate has a much higher angle than in the paper, right? Isn't it possible that lift and drag are strongly time dependent? Looks like you have strong oscillations in the wake...
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2012, 03:00
Default
  #25
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Sorry I was busy for 2 days, I worked on your geometry and I guess I got the good blocking.min quality is 0.8 which is very good but you have to work yourself on the edge parameters and refine/coarsen the mesh in the appropriate areas and finally put BC's and export the mesh in fluent. I am attaching few pics and project files of ICEM
Attached Images
File Type: jpg 1.jpg (89.4 KB, 20 views)
File Type: jpg 2.jpg (91.2 KB, 17 views)
File Type: jpg 3.jpg (98.4 KB, 20 views)
File Type: jpg 4.jpg (98.5 KB, 15 views)
Attached Files
File Type: zip 2D_Flate plate.zip (8.3 KB, 5 views)
Bollonga and mrenergy like this.
cfd seeker is offline   Reply With Quote

Old   October 18, 2012, 03:07
Default
  #26
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Bollonga View Post
Well, Iíve run the case for 0.25 m/s, using the same solver setup and different time steps: 1, 2 and 4 s. Convergence criteria 1e6 as before.
I comment a few things:

1)
Almost no TVR limitation, just a few cells (small vortexs) at some iterations.

2)
Y+ very small, from 0.1 to 1.8. First layer of prism layer should be higher for SWF. (see picture)

3)
Epsilon residuals in some iterations canít go under 1e6.

4) Turbulence intensity drops too fast so close to the inlet. (see picture) Iíve read in the forum that if TI drops too much it means that equilibrium between k and e is wrong because I have too much dissipation, e is over estimated. I guess I need a higher amount of TI in the inlet so I get the desired value at the plate? But if I put too much TI and initialize the solution from the inlet it may start with TVR limitation from the beginning.


5) Lift and drag keep oscillating even if I have left time enough for the flow to run the entire domain for twice (3200s at 0.25 m/s) (see pictures)


Iím gonna try to simulate at the same scale as the reference, with same Re number and try to get a correct y+ value. Once then I'll have to try again the real scale. Any suggestions?


Thanks a lot
If your are fully resolving the boundary layer(wall y+ <=1) then better use Enhanced Wall Treatment instead of wall functions.
One more suggestion...use SST kw model instead of k-epsilon because angle of attack in your case is very high and there is significant amount of flow separation and k-epsilon model does not properly capture separation instead SST kw model is more recommended in such a situation.
Another point....if turbulent viscosity limit is exceeding in few cells then you don't need to worry as long as your lift and drag are in agreement with experimental results

Regards
cfd seeker is offline   Reply With Quote

Old   October 18, 2012, 07:29
Default
  #27
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
@cfdseeker Thank you very match for the files! That will help me a lot to learn more about ICEM.
As this case has a clear separation point at the edge of the plate, is there a big diference between k-e and k-omega?

@rodrigeuzfatz @cfdseeker I've run the case at a smaller scale and almost didn't have any TVR limitations, just few cells away from the plate at some iterations, nothing to worry about.

y+ is still too low, I prefer to coarsen my inflation layer and use a wall function instead of using the enhanced wall treatment in order to reduce computational effort.
Force coefficients don't oscillate as much as they did before, they are still a bit higher than in literature but I guess I have to resolve near wall flux properly before.
I've read something about TI decay in Fluent users guide (7.2.2), there are some equations to estimate k and e from TI decay and distance.

Is there a way to get time-averaged variables along the plate wall? The only way I know to do that is to write an xy-plot file for each time, and then calculate the mean value. However, I need to save many .dat files to have a good resolution.

I'll share further results. Regards.
Bollonga is offline   Reply With Quote

Old   October 18, 2012, 11:28
Default
  #28
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
As this case has a clear separation point at the edge of the plate, is there a big diference between k-e and k-omega?
yes it has been thoroughly discussed in literature that there is a mark difference b/w k-e and k-w.Standard k-e and RNG k-e under predicts separation,Realizable k-e is a bit better in capturing separation but SST kw is best model recommended for this case

Quote:
I prefer to coarsen my inflation layer and use a wall function instead of using the enhanced wall treatment in order to reduce computational effort.
No no don't do it my opinion....Enhanced wall treatment is best in capturing flow separation especially at such high angle of attacks. SST kw by default use enhanced wall treatment. My opinion is to run the case on this mesh(wall y+ <=1) using SST kw model. I am quite sure that you will get much better results in this case
cfd seeker is offline   Reply With Quote

Old   October 19, 2012, 03:34
Default
  #29
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
Okay, I'll try SST k-w model with the finner mesh, the thing is y+ distribution around the plate reaches very different values. There's always a minimum at the stagnation point in the front face and at two corners but there are peaks at the back face and the two other corners that goes over 1 in the finner case (see y+ picture at comment #23)
1) Do I have to get y+<=1 along all the wall? as the case is strongly time dependent, do I have to look at time-averaged y+ or just the maximum?

By the way, these guys get very good results for a vertical plate in the same conditions as me (just a little geometry difference) using k-e with different wall treatments and they don't use a prism layer around the wall.
http://www.waset.org/journals/waset/v61/v61-49.pdf
2) What are they doing that I'm missing?
Bollonga is offline   Reply With Quote

Old   October 19, 2012, 07:48
Default
  #30
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
I've run the case with SST k-w model, no TVR limitations appeared. The problem is I'm still having wrong force coeficients. Time averaged values are the same as in all previous simulations: Cd=2.979 and Cl=-1.071 while literature ones are Cd=1.945 and Cl=-0.708.
I've been looking at Cp distribution at the plate and made the time average over a complete vortex sheddind cycle. I've compared it to literature values and my Cp's at the back face are much lower (see attached pictures), that's why my Cd and Cl are higher. So I must be simulating something wrong at the wake, could it be because of wrong y+ values at the back face? (see picture of instantaneous y+ at Cd max time) What can be the reason for too low pressure at the back face?

Thanks a lot for your help guys
Attached Images
File Type: jpg Cp_mean_CFD.jpg (25.4 KB, 8 views)
File Type: jpg Cp_mean_flat_plate_70_Literature.jpg (29.0 KB, 9 views)
File Type: jpg PS_2D_19_10-5-3.170_y+.jpg (62.2 KB, 9 views)
Bollonga is offline   Reply With Quote

Old   October 20, 2012, 03:37
Default
  #31
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
the thing is y+ distribution around the plate reaches very different values
You don't need to worry about this, its a normal situation. Wall y+ are dependent on wall shear stress and Re. No. As the Re. No is changing along the length of plate so wall y+ will be different at each point

Quote:
Do I have to get y+<=1 along all the wall?
Not really. It should be in between 1 and 5
mrenergy likes this.
cfd seeker is offline   Reply With Quote

Old   October 20, 2012, 03:39
Default
  #32
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Bollonga View Post
I've run the case with SST k-w model, no TVR limitations appeared. The problem is I'm still having wrong force coeficients. Time averaged values are the same as in all previous simulations: Cd=2.979 and Cl=-1.071 while literature ones are Cd=1.945 and Cl=-0.708.
I've been looking at Cp distribution at the plate and made the time average over a complete vortex sheddind cycle. I've compared it to literature values and my Cp's at the back face are much lower (see attached pictures), that's why my Cd and Cl are higher. So I must be simulating something wrong at the wake, could it be because of wrong y+ values at the back face? (see picture of instantaneous y+ at Cd max time) What can be the reason for too low pressure at the back face?

Thanks a lot for your help guys
Are you sure that your case is Fully turbulent and transition is not taking place?
cfd seeker is offline   Reply With Quote

Old   October 20, 2012, 08:28
Default
  #33
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
I'm not pretty sure if transition is taking place. How can I asure that the case is fully turbulent?
I've increased TI from 10% to 25% at the inlet and let the same turbulent lenght scale (TLS) of 9e-4 m and results are the same.
Now I'm running a case with 25% of TI at the inlet but a TLS of 5e-5 m to make it more diffusive to see if something changes.
Bollonga is offline   Reply With Quote

Old   October 20, 2012, 11:14
Default
  #34
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,964
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by Bollonga View Post
Hi

I've refined my mesh and prism layer around the plate (My mesh now has 57920 nodes) and have run the case with the same set-up as before. Results are still the same, TVR limitation appears between 5 and 6s and spreads all over the wake. I attach a picture of TVR at 23.7s. What can be the problem?

I have references that get good results for a coarser mesh and with less computational effort than me.
http://www.waset.org/journals/ijmae/v6/v6-60.pdf
There, flow over a flat plate at 30ļ is being simulated. The plate is 0.15m length and freestream velocity is 15.25m/s. The mesh is finer but it's in similar proportion to my mesh size. The author has 150 divisions in the plate surface and so do I. Can it be a scale issue? Even if my problem is much bigger it requires similar cell sizes?

By the way, y+ seems better now, even too low in some points. I attach the plot.

Thanks for the help!
I think using the hexa mesh will solve your problem. What do you think?
Far is online now   Reply With Quote

Old   October 20, 2012, 11:40
Default
  #35
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,964
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by Bollonga View Post
Hi everybody,

I am simulating a 2D inclined flat plate with an angle of attack of 70ļ. My domain goes 10H upstream (say H is the plate height, H=9.3 m), 20H downstream, 10H up and 10H down.

Velocity at the inlet is 10 m/s. I am using k-epsilon model with TI=10%. I have tried several values for the turbulence length scale (1m, 0.5m, 0.1m, 0.05m) but sooner or later I get turbulent viscosity ratio limited to 1e5 in several cells in the wake. Which should be the value of the turbulent length scale for this case? Also, TI decays too much at some distance from the inlet so I guess I have to use a higher inlet TI to get the appropriate value when the flow reaches the plate.

Iíve tried different approaches Iíve read in this forum like starting with sparlart-allmaras model and change to k-e later, using first order discretization for k and e, reducing TI for some iterations, etc. I always end with the TVR limited to 1e5.

I have also read that mesh quality can be the problem. Is there a relationship between cell size and turbulent length scale allowable?

I put pictures of the mesh, TVR and TI distribution for the 0.05m length scale case. Notice that the flow hasn't reached the outlet yet.


Any comments or help would be really appreciated. Thanks.
Can you tell me the following info:

1. Reynolds number

2. Time step and no of time steps and how you have determined them?

3. How you are making the time-average Cd and Cl. How many time steps and total time you are taking into account for this purpose?

4. How you are ensuring the convergence

5. Domain extent is good enough? Have you made the sensitivity analysis to domain extent?
mrenergy likes this.
Far is online now   Reply With Quote

Old   October 20, 2012, 11:54
Default
  #36
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
Hi far,

I've already solved TVR limitations by scaling the problem and using a better turbulence lenght. k-e standar with standar wall function and k-w with enhanced wall treatment are not showing this limitation.

The problem is both models give too low pressure at the near wake and so drag and lift coeficients are higer than they should be.

I'm now playing with BC for TI(%) and T length scale to see if results change, but force over the plate is not changing so far. I think it may be related to turbulence model or its parameters.

Quote:
Originally Posted by Bollonga View Post
By the way, these guys get very good results for a vertical plate in the same conditions as me (just a little geometry difference) using k-e with different wall treatments and they don't use a prism layer around the wall.
http://www.waset.org/journals/waset/v61/v61-49.pdf
Here you can see that a relative coarse mesh with k-e gives good results for a vertical plate.

Thanks
Bollonga is offline   Reply With Quote

Old   October 20, 2012, 11:59
Default
  #37
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,964
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
I've already solved TVR limitations by scaling the problem

What do you mean by scaling the problem?
Far is online now   Reply With Quote

Old   October 20, 2012, 12:15
Default
  #38
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
I've just seen your last comment.

1) Re no is 1.55e5 (plate length=0.15m, u=15m/s)

2) I've tried several timesteps: 5e-4, 1e-3, 2e-3 and eventually I'm using 25e-4. I let the flow goes several times all along the domain (6.25 m long) that is 800 timesteps. But I've have checked that mroe iterations don't change the result.

3) Once the coefficients are constante I've measured the period of a cycle of lift and drag force, they are almost 0.07s and I've writen a Cp file every 0.001s. I've made the average for each point and got the time-averaged Cp distribution for a complete cycle.

4) Residuals are 1e-5.

5) Now it's 41.6*L long and 27.7*L where L is the plate length 015m. I've tried a larger one and results are the same.
3)
Bollonga is offline   Reply With Quote

Old   October 20, 2012, 12:45
Default
  #39
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
What do you mean by scaling the problem?
By scaling I mean to reduce the scale of the mesh.
My real plate is 9.13m but I wanted to compare with literature experiments for a 0.15m plate. So I reduced mine to have the same length.
The real scale problem gave TVR limitation but the same mesh with reduced scale gave no problem.
Bollonga is offline   Reply With Quote

Old   October 20, 2012, 13:00
Default
  #40
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,964
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What is the value of density and viscosity and why you choose these values?

How did you determine the time step size? Is it according to any method available in literature?

Do you wanna try the hexa mesh? I have made one. In this mesh, Y+ is 1 (good for transition model as well) but requires more time steps. You may need the transition model for better prediction of Cd.




mrenergy likes this.
Far is online now   Reply With Quote

Reply

Tags
3d 2d, flat plate, turbulence models, viscosity limitation

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
Turbulent viscosity ratio limited to 1.10^5 in boundary layer ingestion loicflouriot FLUENT 0 May 27, 2012 07:31
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Problem of Turbulent Viscosity Ratio Limited David Yang FLUENT 3 June 3, 2002 06:13


All times are GMT -4. The time now is 02:09.