# Ahmed body -Drag coefficient not converging!!

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 January 12, 2014, 09:50 Ahmed body -Drag coefficient not converging!! #1 New Member   Join Date: Jan 2014 Posts: 7 Rep Power: 12 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.

 January 12, 2014, 21:59 #2 Senior Member   Join Date: Feb 2013 Location: Germany Posts: 200 Rep Power: 24 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.

 January 13, 2014, 04:35 #3 New Member   Join Date: Jan 2014 Posts: 7 Rep Power: 12 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

 January 13, 2014, 08:39 #4 Senior Member   Join Date: Feb 2013 Location: Germany Posts: 200 Rep Power: 24 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. .

 January 13, 2014, 22:31 #5 Member   Join Date: Dec 2012 Posts: 92 Rep Power: 13 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

 January 14, 2014, 07:54 #6 New Member   Join Date: Jan 2014 Posts: 7 Rep Power: 12 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

 January 14, 2014, 08:28 #7 Member   Join Date: Dec 2012 Posts: 92 Rep Power: 13 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

 January 14, 2014, 08:29 #8 Member   Join Date: Dec 2012 Posts: 92 Rep Power: 13 Oh btw: Is the model 3D or 2D?

 January 14, 2014, 09:22 #9 Super Moderator     Alex Join Date: Jun 2012 Location: Germany Posts: 3,406 Rep Power: 47 I bet 10\$ that the simulation will converge once you run more than 700 iterations

 January 14, 2014, 14:00 #10 New Member   Join Date: Jan 2014 Posts: 7 Rep Power: 12 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

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Ketut Utama Main CFD Forum 8 December 11, 2014 11:03 jackwabbit STAR-CCM+ 2 September 2, 2013 04:36 haghgoo_reza OpenFOAM Running, Solving & CFD 0 April 25, 2013 16:35 Jhonathan CFX 2 October 2, 2008 18:07 ace FLUENT 2 January 27, 2004 10:14

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

 Contact Us - CFD Online - Privacy Statement - Top