CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

very low drag and lift values

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

Like Tree2Likes
  • 1 Post By fluid23
  • 1 Post By fluid23

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 13, 2016, 13:07
Post very low drag and lift values
  #1
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
Hello, i'm simulating a frontwing with a rotated tire and the results i get are very weird.
I use the surface wrapper and surface remesher, because the part has many errors.
But the pressure and vectors look good.
Attached Images
File Type: jpg FF mit Gurney_Cl Plot.jpg (92.8 KB, 37 views)
File Type: jpg FF mit Gurney_Cd Plot.jpg (87.6 KB, 22 views)
File Type: jpg FF mit Gurney + Reifen_Druckverteilung (Isometrieansicht).jpg (33.5 KB, 43 views)
File Type: jpg FF mit Gurney + Reifen_Vector.jpg (59.2 KB, 32 views)
File Type: jpg FF mit Gurney_Residuals.jpg (88.1 KB, 21 views)
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 13:18
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
Well, first of all it appears that you have some unsteady phenomenon. You should consider using the implicit unsteady solver. The sinusoidal waves in your residual and force curves are a result of this. That will help some.

My next question is whether your wall y+ values are appropriate for your turbulence/wall model. Followed by are the inputs into your force coefficient reports correct (i.e. reference area, density, velocity?).
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 13:40
Default
  #3
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
thats my setup and the residuals going wild when i choose the implicit unsteady solver, but the drag and lift values stay constant

i don't know what to do
Attached Images
File Type: png physics setup.PNG (28.8 KB, 32 views)
File Type: jpg Residuals2.jpg (88.6 KB, 30 views)
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 13:59
Default
  #4
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
It looks like you aren't letting each time step converge. Try adding more inner iterations and see if things calm down a bit. You should expect to see a spike in residuals at each new time step after which they will reduce and converge if things are setup properly.
dennis722 likes this.
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 14:19
Default
  #5
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
the residuals looks better after unenable the maximum inner iterations, but the drag an lift results are as low as at the beginning

between 1350-1400 iterations i have tested something this doesn't matter
Attached Images
File Type: jpg Results3.jpg (99.0 KB, 24 views)
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 14:21
Default
  #6
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
Ok... so what about the other issues I mentioned. Wall y+ and force coefficient report inputs?
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 14:33
Default
  #7
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
the force coefficient report is correct, but i never worked with the wall y+ values
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 14:36
Default
  #8
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
Are you sure that your reference area is appropriate? Maybe try looking at the forces rather than coefficients to get a sense of whether they are correct. How do you know that they are wrong at present? Do you have feel for what they should be or are you trying to duplicate experimental data or published results?

As for wall y+, that is at the core of everything you are trying to do, especially on drag values. I suggest looking into this more. Based on your turbulence and wall model selections I would target 1-5 or 30-60, but anything between 5-30 will also be ok, just a little less accurate.
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 14:52
Default
  #9
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
i have uploaded the settings of my plots and the coordinate system of my simulation

i think the Cl and Cd values are too low, because normally frontwings like this doesn't have such low values. I looked at some comparable worth in the internet
Attached Images
File Type: png Cd.PNG (16.1 KB, 20 views)
File Type: png Cl.PNG (17.8 KB, 19 views)
File Type: png frontal area.PNG (34.5 KB, 18 views)
File Type: png mesh.PNG (50.2 KB, 31 views)
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 15:08
Default
  #10
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
I suspect that your reference area choice is not correct. I don't know a lot about car aerodynamics but I do no a good bit about airplane aerodynamics and I would never choose a wetted surface area as a reference area. You typically want to choose a 'planform' area.

For example, a rectangular aircraft wing would use A= span * chord. Using wetted surface area will make your reference area more than twice what it should be.

That being said, I calculated the actual force from your plot and settings and I am getting around 60 N. That does seem a bit too low. The comparable values you are seeing on the internet, what do those show?
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 15:09
Default
  #11
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
Oopps... sorry. I see now that you used frontal area. That may be more appropriate assuming it was setup correctly.
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 15:17
Default
  #12
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
I have changed the reference area and now i have a Cd=0,345 and a Cl=-0,775 which is much more relastic
I think the parts i choosed in the frontal area report were wrong, because i took the regions without the ground, inlet,outlet and symmetry planes as the parts.
Now i have set my directly my assembly as the part for the frontal area


and back to the y+ values where can i chance the value in star ccm+? i only find that i can set it to high or low y+ values in the solver
Attached Images
File Type: png frontal area2.PNG (15.2 KB, 23 views)
dennis722 is offline   Reply With Quote

Old   July 13, 2016, 15:40
Default
  #13
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 847
Rep Power: 14
fluid23 is on a distinguished road
Wall y+ isn't a value you choose, it is a product of your mesh. It is a non-dimensional distance that you use to judge whether your near wall cells are sized properly. For sizing of wall y+ for a given flow I would refer you here...

http://www.cfd-online.com/Wiki/Dimen..._wall_distance

Your goal is to get a mesh that results in wall y+ values that are appropriate for the wall model and turbulence model you choose. For k-e with all wall y+ model you will want to have between 1-5 or 30-60 for best accuracy. Independently these ranges are the 'low' and 'high' wall treatments. The all wall y+ model will effectively interpolate between low and high wall models for values that are between 5-30... this will result in some error, but probably not anything that you are worried about give the scope of your effort. So... shoot for 1-60 for wall y+ and you will be fine.

You will have to let the model converge (or at least get very well established) then examine a scalar scene with all wall boundaries as input parts and field function set to wall y+...

This should get you started, there is more to it than that so I strongly encourage you to read and understand what wall y+ is, how it is used and hopefully realize that it can NEVER be ignored.
dennis722 likes this.
fluid23 is offline   Reply With Quote

Old   July 13, 2016, 15:47
Default
  #14
Member
 
Dennis
Join Date: Jul 2016
Location: Germany
Posts: 37
Rep Power: 6
dennis722 is on a distinguished road
Thank you very much for your answers! I will take a closer look to the y+ values and try to understand it
dennis722 is offline   Reply With Quote

Reply

Tags
drag, error, lift, low, wrapper

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
wrong SU2 calculation for lift and drag coefficient for NAC4421 mechy SU2 7 January 9, 2017 06:18
Lift Drag and Reference Values in 2D kike FLUENT 0 July 9, 2015 18:52
Oscillating residual, lift and drag values aptahaney Main CFD Forum 0 July 8, 2015 14:16
Lift and Drag Monitor Point Values Converging to Zero Josh CFX 24 May 9, 2011 11:38
Correct values of drag but high values of lift. aamer Main CFD Forum 16 December 16, 2010 05:44


All times are GMT -4. The time now is 13:18.