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

Ahmed body -Drag coefficient not converging!!

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

Like Tree1Likes
  • 1 Post By sam92

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 12, 2014, 09:50
Default Ahmed body -Drag coefficient not converging!!
  #1
New Member
 
Join Date: Jan 2014
Posts: 7
Rep Power: 12
sam92 is on a distinguished road
Hi All,
I am trying to simulate flow around an ahmed body with 35 degree slant.I have been following some tutorials online , but my drag coefficient is not converging.Below is an overview of the meshing and simulation details I have used.

MESHING

Total number of elements -2.9 million approx
Min size-1mm
Max size-250mm
Minimum edge length-50mm

I have added face sizing and rear body sizing with 8mm element size
5 Inflaton layers for the body and road with growth rate of 1.2 , following smooth transisition

SIMULATION

Boundary condition:- inlet velocity-40m/s ,outlet -atmospheric presure and no slip for road and body, rest all symmetry planes

Pressure based solver,steady state
realisable k-e ,non-equillibrium wall functions

Coupled scheme, gradient- least square cell based
First order upwind for momentum,k,e for first 100 iterations then changed to second order.

courant number-50, relaxation of 0.25 for momentum,pressure and 0.8 for rest

standard initialization based on velocity inlet

i have done about 700 iterations and my drag coeffiecient seems to be increasing and decreasing around .28xx

I have attached a snapshot of the residuals

If someone could please give me some insight to where i went wrong,it would be really appreciable.

Thanking you,
sam92

ahmed_mesh.png

ahmed1_mesh.png

cd-history.txt

residuals.jpg
wuttibhat likes this.
sam92 is offline   Reply With Quote

Old   January 12, 2014, 21:59
Default
  #2
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 200
Rep Power: 24
kad will become famous soon enoughkad will become famous soon enough
Generally oscillation is a typical behaviour of 2nd order schemes when gradients are not resolved good enough. You can try to refine the mesh in areas of high gradients.

Looks like you followed the detailed tutorial for ahmed body in workbench on youtube . Also check FARs tutorial especially for hexa meshing of ahmed body. http://www.youtube.com/watch?v=2baEa...ature=youtu.be
This should give you a way better mesh.

Further I personally would start with hybrid initialization, default URFs, double precision solver and use k-omega-sst model. Further iterate way more than 700 iterations.
kad is offline   Reply With Quote

Old   January 13, 2014, 04:35
Default
  #3
New Member
 
Join Date: Jan 2014
Posts: 7
Rep Power: 12
sam92 is on a distinguished road
Thank you for your reply kad.
I'll try to refine my mesh near the regions of high gradients and see how further iterations go.
Should i use default URF's or go ahead with the URF's I was using?

Thanks a lot
sam92 is offline   Reply With Quote

Old   January 13, 2014, 08:39
Default
  #4
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 200
Rep Power: 24
kad will become famous soon enoughkad will become famous soon enough
I would try default URFs first. If your solution is not converging you can change them later. As mentioned before I would also switch to k-omega-sst turbulence model. The k-epsilon model does not perform well in areas with stagnating or separating flow. Both of these phenoms occur in your model and should have significant influence on the drag value. .
kad is offline   Reply With Quote

Old   January 13, 2014, 22:31
Default
  #5
Member
 
Join Date: Dec 2012
Posts: 92
Rep Power: 13
beer is on a distinguished road
Did you have a look at the solution?
It is probably not really a convergence problem. If the flow around your body is just transient (vortex street etc.) your residual won't go down at all. You could suppress these effects with relaxation, but that actually makes your solution wrong.
For example have a look at a cylinder with and without Karmann vortex, the difference for the drag is around 45%. (around 1.3 in transient and 0.9 in steady I think).
Anyway consider maybe using a transient simulation and average the solution.
I'd be interested if you can solve it with that so please let me know if you tried it

Cheers
beer is offline   Reply With Quote

Old   January 14, 2014, 07:54
Default
  #6
New Member
 
Join Date: Jan 2014
Posts: 7
Rep Power: 12
sam92 is on a distinguished road
Thanks for your suggestions beer

But in the tutorial's online, a steady state simulation was performed on ahmed body(25 degree slant) with realisable k-e model and the obtained drag coefficient was within 5% of the experimental value.

The only difference is that i am doing the simulation on a 35 degree slant one,rest all the steps are the same as the tutorial.

I've found that for the 35 degree case there is detached flow over the slant compared to attached flow for 25 degree case.Is that why the k-E model is failing in my case?


I'll try doing a transient simulation, if someone could share their transient simulation setup details, it would be really helpful.

Thanks a lot
sam92
sam92 is offline   Reply With Quote

Old   January 14, 2014, 08:28
Default
  #7
Member
 
Join Date: Dec 2012
Posts: 92
Rep Power: 13
beer is on a distinguished road
Hm, ok this is still possible. Detachement is exactly what I mean. After an detachement you have recirculation which can lead to transient effects which affect your convergence. But I can't really say from here if this is the problem. Like I said, just try a transient one with 10-20 inner iterations and you should see after a few iterations if the timesteps converge. If yes, it is very likely that your flow is just "too transient" for your steady state solver.
If not you have to dig a little bit more. It could be still also the mesh, the boundary conditions, solver parameter etc. etc...

Cheers
beer is offline   Reply With Quote

Old   January 14, 2014, 08:29
Default
  #8
Member
 
Join Date: Dec 2012
Posts: 92
Rep Power: 13
beer is on a distinguished road
Oh btw: Is the model 3D or 2D?
beer is offline   Reply With Quote

Old   January 14, 2014, 09:22
Default
  #9
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,406
Rep Power: 47
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
I bet 10$ that the simulation will converge once you run more than 700 iterations
flotus1 is offline   Reply With Quote

Old   January 14, 2014, 14:00
Default
  #10
New Member
 
Join Date: Jan 2014
Posts: 7
Rep Power: 12
sam92 is on a distinguished road
The model is a 3d one.

As flotus 1 said ,I'll iterate it further to see if the drag coefficient converges .

Also,As kad pointed out, i'll look into whether a mesh refinement at areas of high gradients solves the problem and let u know.

If both the above doesn't work, I guess a transient simulation or using a different turbulence model(like SST) is the only option I have.

Thanks a lot
sam92
sam92 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
Drag Coefficient for Ellipse Form (2D) Ketut Utama Main CFD Forum 8 December 11, 2014 11:03
Ahmed body drag coefficient jackwabbit STAR-CCM+ 2 September 2, 2013 04:36
Drag coefficient on a 2-D cylinder haghgoo_reza OpenFOAM Running, Solving & CFD 0 April 25, 2013 16:35
How find Drag coefficient of a body with ANSYS CFX Jhonathan CFX 2 October 2, 2008 18:07
to find drag coefficient of an ogival body ace FLUENT 2 January 27, 2004 10:14


All times are GMT -4. The time now is 17:06.