# Problem with convergence residual

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

April 30, 2011, 12:00
Problem with convergence residual
#1
New Member

Tom Janda
Join Date: Apr 2011
Location: Czech
Posts: 7
Rep Power: 8
Hi, I´m student, now I´m working on my thesis work on topic Car body. I have problem with value of residual.

I created model of sports car (half model exactly) and wind tunnel (size tunnel: 7 metres width, 6 metres high, 90 length). This all was imported to Star-ccm+. Mesh have 1 241 000 cells (polyhedral).

Flow conditions are: Three dimensional, Gas, Cell quality remediation, Coupled flow, Motion are stationary, Constant density, Time is steady, Viscous regime was selected Turbulent, Reynolds - Averaged Navier Stokes, K - Omega turbulence, SST (Menter) K-Omega, All y+ Wall Treatment.

On the start of tunnel is condition: velocity inlet (28 km/h, and in the end of tunnel is condition pressure outlet (0 Pa). Car and road have condition Wall, other side of tunnel have condition Symmetry.

Program calculted residuals as you can see on picture. I read somewhere about boundary of convergence is to be 10-4. During 800 iterations curves residual are decreased, and after were not change to the 2800 iteration. Then I stopped it . I´m tried change turbulent flow on laminar on 2850 iterations. I´m tried show of flow (pics enclosed), and I don´t know if the results with this mistake residuas can be right. My computer calculated this results 2 days, approximate numb is 50 iteration/hour (Pentium i3, 8gb ram)

Attached Images
 Streamlines8 - Kopie.jpg (82.2 KB, 303 views) Residuals - Kopie.JPG (52.2 KB, 461 views) 11 - Kopie.JPG (91.6 KB, 343 views)

 April 30, 2011, 17:38 #2 Member   Join Date: Apr 2011 Location: US Posts: 43 Rep Power: 8 Come on, your total mesh size is too small comapred to your geometry. And you were using your own computer to run the simulation.....

 May 1, 2011, 07:20 #3 Senior Member   Join Date: Oct 2009 Location: Germany Posts: 637 Rep Power: 15 I'm feeling like a scratched record, I'm writing the same again and again: You shouldn't give too much on the residuals. They are normalized during the first 5 iterations and therefore the final level strongly depends on the initial values. Further you can see some oscillations in the residuals. That's an indicator for a unsteady nature of the flow while you are running the case steady state. That might be another reason why residuals drop less than you expected. That should not mean "you have to run it unsteady", that should mean "don't give too much on residuals". And further I have to agree to famerfamer. The mesh is way to small to capture all flow phenomena. Just to give you an order of magnitude, a F1 car usually has about 100 Million cells, and even that still gives no mesh-independend solution. Anyway, that much will not be realistic for you, but your machine can handle at least six times as much as you are using now. I now, that will slow down your simulation, but that's how CFD works - using much computational power or waiting for ages. Two other things that came into my mind: Have you applied rotation on the tyres and motion on the ground? How does the contact between tyres and road look like?

May 1, 2011, 08:05
#4
New Member

Tom Janda
Join Date: Apr 2011
Location: Czech
Posts: 7
Rep Power: 8
Hi abdul099, thanks for asnwer,

I tried rotation on tyres, motion on road I applied too (I forgot to upload). Mesh size of car is 22 mm, and I diluted the size of the tunnel elements by 7 blocks. (firts block mesh size is 50 mm, next 100, next 200, ... and last block have mash size 500 mm). I have to do somothing correction on design car body, so I need more accurately results. I proceeded through the thesis work of my teacher and there is written about the conditions convergence as I wrote. Now I tried to change the length the tunnel on 55 metre (from 90 metres). The residual curves increased a lot too (attached screen).

Don´t you have any idea? If I understood correctly, there is the problem with number of cells car compared the cells tunnel? My teacher told me that I can´t get number 2 milions cells.
Attached Images
 Streamlines3 – kopie.jpg (85.5 KB, 133 views) Výstřižek4 – kopie.JPG (33.6 KB, 146 views) bad_residual.JPG (49.0 KB, 237 views)

 May 1, 2011, 09:46 #5 New Member   Tom Janda Join Date: Apr 2011 Location: Czech Posts: 7 Rep Power: 8 I thought if I don´t fault in the direction speed of the road. I changed direction road speed against the direction of the x-axis. Before it was reversed. And the direction rotation tyres it was the same. I also change (direction rotation tyres).

 May 1, 2011, 11:14 #6 Senior Member   Join Date: Oct 2009 Location: Germany Posts: 637 Rep Power: 15 Why can't you get even up to 2 million cells? Of course, it will take longer, but without an appropriate mesh resolution, you will not get good results. For me it sounds like "uh, I need a car with a top speed of 300km/h. But the 5l V8 needs to much fuel, so let's try it with a scooter engine. When it doesn't reach the desired top speed, let's complain in a forum, for sure some smart guy will have some hints how to tune the scooter engine to reach a top speed of 300km/h". It's up to you what mesh size you're using - but no hint can make a miracle to occur. To judge convergence, you shouldn't bother about residuals which decrease not enough or maybe increase a little bit. As I mentioned before, the residuals are normalized within the first 5 iterations. Imagine, you would initialize with a "perfect" solution, therefore the non-normalized residuals would be very low. When starting the simulation from that perfect state, the residuals are normalized and they will never drop. So you can't judge convergence just by looking on the residuals! You should have some plots for drag, lift or whatever value you are interested in. Look at this plots, when they reach a continous level and the residuals have stabilized (at what level ever), you can stop your simulation. In general, I would use the longer wind tunnel. The cells can grow a lot towards the end, so the impact on the cell count will be very low. It's also necessary to dissipate eddies, pressure changes etc. before they reach the outlet which will be done by the growing cells. fshak92 likes this.

 May 1, 2011, 11:49 #7 New Member   Tom Janda Join Date: Apr 2011 Location: Czech Posts: 7 Rep Power: 8 Ok, I understand what you mean. Now I run the calculation, but the program reports me message on output message: Outlet: reversed flow on 17 faces. I think that I have short tunnel (90m). I will try to increase length tunnel at 200 meters, for sure. Thanks for your advice Regards, Tom.

 May 1, 2011, 13:47 #8 Senior Member   Join Date: Oct 2009 Location: Germany Posts: 637 Rep Power: 15 Reversed flow is not that problematic, but you can also prevent it by increasing the cell size near the outlet. This will dissipate vortices etc. which I assume are the cause for the reversed flow at the outlet. Good luck

May 1, 2011, 15:43
#9
New Member

Tom Janda
Join Date: Apr 2011
Location: Czech
Posts: 7
Rep Power: 8
Quote:
 Originally Posted by abdul099 Reversed flow is not that problematic, but you can also prevent it by increasing the cell size near the outlet. This will dissipate vortices etc. which I assume are the cause for the reversed flow at the outlet. Good luck
Last question, I´m sorry, that I ask so stupidly. Can I ask what sign would you choose for direction the rotation tyres and road speed to coordinate system? x-axis is directed against the direction ride, y -axis is directed to the center car.

I opted for the speed of the road a positive sign, this means that the speed of the road has the same direction as the x-axis. Direction of velocity has a negative direction (-90,032 rad). I used the enclosed picture. These directions are as I think it should be. So that now computing.

In thesis works other students is the x-axis is directed in the direction ride, y -axis is directed to the center car. But they have positive sign, as rotation of the wheels and direction of the road. So they have the opposite sign than I when now. When I followed the same principle as they are, so it suited me message: reversed flow.

So what rate ( + or - ) the road sign would you choose? (to boundary) This is last question, perhaps. Tom
Attached Images
 reversed_flow – kopie.JPG (55.3 KB, 120 views) reversed_flow3 – kopie.JPG (30.3 KB, 117 views) wind_tunnel_roll_belt.gif (37.9 KB, 113 views) rychlost_kol – kopie.JPG (64.8 KB, 109 views) rychlost_vozovky – kopie.JPG (70.4 KB, 84 views)

 May 3, 2011, 03:30 #10 Senior Member   Join Date: Oct 2009 Location: Germany Posts: 637 Rep Power: 15 The velocity of the road seems reasonable to me. It simply the opposite direction the car would travel, therefore the opposite direction of the incoming flow (when running without yaw). To get the wall rotation of the tyres, use the right-hand rule. Point your thumb in the same direction as the desired rotation axis which will be the Y-axis (positive direction of Y!) in your case. Now the curvature of your relaxed fingers will show you in which direction the wall would rotate when a POSITIVE rotation rate would be applied. In your case, this is obviously the wrong direction, as the tyres would rotate against the road. Therefore a negative rotation rate is necessary in your case. You already did it right. It's possible to check it by plotting not the velocity magnitude in the scalar scene but the velocity in X-direction. What diameter do your tyres have? I'm just wondering about the rotation rate.

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post richard OpenFOAM Running, Solving & CFD 168 November 14, 2017 12:51 cyberbrain OpenFOAM 4 March 16, 2011 10:20 vw.cfd OpenFOAM 6 August 7, 2009 05:44 paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 22:14 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58

All times are GMT -4. The time now is 14:57.