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

 March 9, 2004, 07:11 Re: Please help with flow around car modelling! #2 Tudor Miron Guest   Posts: n/a Hi All, I allready figured that model came in "scaled" - became a very little tiny thing . It was created in SolidWorks using inches. I imported it again and this time left database units as default. In Build when in geometry I choused inches and when created a point with inch aoordinates it apeared where it had to. I'll rerun the model now and will report the results. Still have main questions: What IS the correct conditions to model flow around car body. Any hints and suggestions will be highly appritiated. One persone from Ford Racing (he was not doing CFD but was supervising all project) told me that it took me two! years to come up with model that corelated with wind tunnel testing.... That makes me worryed... Does it mean that CFD is useless (race car aero)if I don't have wind tunnel handy to corelate results? I really hope that this is not the case... Thank you Ted

 March 9, 2004, 09:43 Re: Please help with flow around car modelling! #3 Tudor Miron Guest   Posts: n/a I reruned the model with coarse mesh (221000 nodes)and when in SFXC-Post got more realistic numbers. L = 1262[N], D = 115.108[N]. This was not a model of real car but a blunt body with inclouded tunnel. Small frontal area 0.12m^ (1.34ft^) and kind of inverted airfoil shape running close to the ground suggest that this numbers might be slose. When tryed to calculate Cd I thought that I should take "plane" area as is used when calculating Cd of airfoils. So Cd = D/(0.5 x 1.22 x 44.44^ x 1.94) = 0.047 I don't know if it sounds realistic for such a model. If I calculate it using frontal area than I get Cd = D/(0.5 x 1.22 x 44.44^ x 0.12) = 0.79. Ld using same formula = -0.54 How ever when I calculated area of model it showed 4.8M^ and SolidWorks where model was made shows 5.01M^ ... Difference is not THAT big but still it's confusing Any suggestions will be highly apreciated. Thank you Ted PS: Sorry for my English and dumb questions - but there's nowhere also to ask - please help.

 March 9, 2004, 17:57 Re: Please help with flow around car modelling! #4 Glenn Horrocks Guest   Posts: n/a Hi Ted, It does not surprise me it took a guy from Ford Racing two years to get good agreement. A good model of something as complex as car external aerodynamics is a very difficult assignment. That does not mean CFD is useless without wind tunnel data, it just means you need to do some homework. Wind tunnel data is very useful if you can do it, but if you can't you should look at the literature. The main foundation paper in this field was done by Ahmed (hence the Ahmed body). It forms the basis of one of the tutorial problems in CFX 5.6. I think there is a reference to this paper in the documentation. Get a copy of this paper, and try to reproduce his results. Many authors since then have used this shape to benchmark the accuracy of their simulations since then, so you should also be able to uncover many more recent papers using the same model. Also look for literature on car aerodynamics in general. There's lots of published works on this topic out there. Glenn

 March 10, 2004, 07:05 Re: Please help with flow around car modelling! #5 Tudor Miron Guest   Posts: n/a Hi Glenn, Thanks a lot for your help. While I found some resent SAE papers referring to Ahmed body: 2004-01-1308, 2004-01-0442, 2002-01-3349, 2001-01-2742, 942498 I could not find Ahmed's paper itself. Could you please give its number or full name? Also are there any other papers that you would recommend? Also I have some more dumb questions: 1) Is Physical timescale 1/3 of time that fluid takes to flow through domain good enough? Could I use automatic timescale? 3) Currently I'm setting simulation as steady-state, is it proper way? 4) What is proper convergence target? 1e-4? 1e-6? I've heard from one person that decent results can be had with 1e-3… that would be nice 5) What turbulence (SST) options should I use? Currently I was using Medium 5%. 6) As indicated in earlier posts I had problems (dimension wise) when importing iges file to Build. Even now when model is close to it's CAD size, calculating "area" in CFX-Post I get slightly different numbers than in SolidWorks for same model – any suggestions. Thank you very much for you help! Your input is invaluable and highly appreciated. Thank you Ted

 March 10, 2004, 17:01 Re: Please help with flow around car modelling! #6 Glenn Horrocks Guest   Posts: n/a Hi Ted, On the CFX community page there is an extended Ahmed body example where they give the full reference: http://www-waterloo.ansys.com/cfxcom...Ahmed_Body.htm To answer your questions: 1) In a steady state flow, adjust the timestep to give best convergence speed. Don't be too worried about it, if you don't have the optimum number you will just have to do a few more iterations to get to convergence. 2) Question seems to have disappeared! 3) If you are looking for the time averaged response, then yes. As long as it converges acceptibly this will do. If you are interested in the vortex shedding off the back or are having convergence problems then no. 4) Convergence levels are discussed in the following document: http://www-waterloo.ansys.com/cfxcom...onvergence.htm 5)I assume you are talking about initial and inlet turbulence conditions. The initial turbulence condition does not matter as it gets blown away during the simulation (as long as it is not too wildly off then it won't converge). The inlet turbulence levels are dependant on what you are trying to model - for instance a windy day or other vehicles in the vicinity. Also, often the inlet turbulence levels do not make a huge difference to the answer (but sometimes they do!). 6) CFX-Post will give slightly different values for volumes and areas as it is calculating it based on the discretised shapes, that is the shape of the elements. SolidWorks hopefully uses the exact geometry. Regards, Glenn

 March 10, 2004, 21:07 Re: Please help with flow around car modelling! #7 Neale Guest   Posts: n/a Answers to your questions: 1. 1/3 is pretty good. If you experience robustness problems then 1/4-1/5 may be necessary. The rule is use the biggest timestep you can get away with. 3. Probably steady state is just fine for lift/drag, unless you are interested in simulating transient vortex shedding off the geometry or something. 4. Read the convergence doc already pointed out by Glenn. 1.0e-3 MAX is good for ballpark solutions and 1.0E-4 should be used if you want "final" results. 5. SST is a pretty good choice. To get best results though you need a really good boundary layer grid with at least 5-10 prism layers in the boundary layer. Inlet turbulence levels usually don't have to be touched. However, in some cases, if you are running a domain where the inlet is *far* upstream of the car then the turbulence can die out by the time it reaches the car and the flow is essentially running laminar around the car. This usually results in non-convergence or robustness problems which it sounds like you are not having. In addition, you might for interest also read through the CFX Validation report or DES: http://www-waterloo.ansys.com/cfxcom...on/default.asp It discusses Ahmed body results. The focus is DES but they also used SST and other models as well. Neale

 March 11, 2004, 16:13 Re: Please help with flow around car modelling! #9 Glenn Horrocks Guest   Posts: n/a Hi Ted, With respect to your different residuals and the lift and drag they predict: As the lift, and especially the drag is still moving around with different convergence levels, this indicates that you have not yet reached a properly converged solution. 1) Your tightest convergence is 1e-5 (RMS) which is pretty tight, but the problem with RMS residuals is there can be a small region of high residuals which get offset by the far greater region of lower residuals resulting in premature convergence. I bet the local high residuals are in the wake region behind the car, and this region would have a large effect on the L & D figures. I would recommend repeating with MAX residuals. 2) You may not be reaching a fully converged solution because of a grid problem. Almost always this means your grid is too coarse, especially in the "difficult" region, which is the rear of any bluff body where the seperations occur. If you can, try a finer grid. Regards, Glenn

 March 11, 2004, 16:36 Re: Please help with flow around car modelling! #10 Tudor Miron Guest   Posts: n/a Thank you Glen, I don't have much more CFX time tonight so could you please point me: should I first refine the mesh or should repeat with MAX residuals first. Also to my shame I don't know how to repit with max residual Thank you Ted

 March 14, 2004, 07:21 Re: Please help with flow around car modelling! #11 Bob Guest   Posts: n/a Hi Ted, to set the maximum residuals you set them in the solver control section, you should be able to see the GUI set to RMS residuals and a value. If time is an issue then always better to go for the faster option, ie in your case change the residuals, as chjanging the mesh will take some time and you may not have anything to run when your time is up ! Another suggestion is to monitor the forces on your basic car shape. If you have a wall boundary condition defined that covers all of your car surfaces and nothing else, you can then monitor the forces on this boundary condition. To do this goto the solver manager and create a new monitor trace (not sure what they call this officially as I'm not infront of a CFX machine), then right click on the window, and choose the monitor properties, and pich the forces option. There you will be able to pick the stream wise force and also the vertical force for that boundary. These traces will give you a feel for how well the drag and lift are converging. Hope this helps and sorry for not being able to remember the exact names of some of the GUI's Bob

 March 15, 2004, 16:23 Re: Please help with flow around car modelling! #12 Tudor Miron Guest   Posts: n/a Thank you Bob, How ever for a day or two I woudn't be able to work with CFX. My sun is ill so I can't stay late at work. But I'll try your suggestions as soon as I get to CFX machine. In the meantime I'd like to ask if someone will take a look at "physics conditions" I'm aplying in PRE for this problem - does it look right? Also as Neal stated to get advantage of SST model I should have at list 5 layers within boundary layer. Question is HOW DO I KNOW how many layers I have? Again sorry for dumb question. Thank you Ted

 March 17, 2004, 15:15 Re: Please help with flow around car modelling! #14 Tudor Miron Guest   Posts: n/a Thank you Neale, First I have to say that I do know how many prism layers I have as I set them myself…. But how do I know how many I have within a boundary layer? Or I'm overenthusiastic here? I thought that CFX manual wanted me to have at list 5 – 10 layers WITHIN boundary layer… they never told should it happen at front or rear section of car …. Now to convergence problems that I had. I really think that this was those 2600 flat tetrahedral elements that outfile "noticed". Refining mesh control to 7.5mm didn't help. What did help is reducing number of inflation layers from 20 to 5. This left me with only 3 flat tetra elements and solution converged to 1E-04 nicely. How ever I think that this was a problem in fairly small bit of mesh as force results was very close in previous run (one fluctuating at 1E-4.8 for about 50 iterations and last one) but this is bothering me…. I would really like to find solution for this kind of problems (fixing the mesh) without reducing number of layers. One guy told me that in this case I should run a transient solution – he says that otherwise fluctuations can not be solved without coarsening the grid…. Never tried a transient yet. It was stated in this thread that I don't need transient unless I want to study vortex shedding off the rear of car model. I actually very interested in accurate vortex prediction as it plays major role in my underbody aerodynamics – I'm trying to do something similar as older group C cars. Any suggestions? Also I'd like to ask is there some rule of thumb for fluid domain size when working on automotive solutions? Thank you Ted

 March 17, 2004, 16:36 Re: Please help with flow around car modelling! #15 Glenn Horrocks Guest   Posts: n/a Hi Neale, ted, You will have to get rid of these flat elements before it will converge nicely. Forget about transient issues, RMS/MAX convergence and everything else until you have a grid with no flat elements. Have a look at my other posting on this issue, hopefully it can help you get rid of the flat elements. Glenn

 March 17, 2004, 17:10 Re: Please help with flow around car modelling! #16 Tudor Miron Guest   Posts: n/a Even if I have only 4 flat elements in 1700000 elements grid?!?! Is it that important? Any way I'm off to read your post on this issue. Thank you Ted

 March 18, 2004, 16:44 Re: Please help with flow around car modelling! #17 Glenn Horrocks Guest   Posts: n/a Hi Ted, Yes, it is important. Sometimes you can still get it to converge, but sometimes not. Either way, convergence will be much faster and more reliable without them. The MAX residuals are the maximum residual in the simulation, and that is likely to occur at the flat element so it is likely to be the area slowing convergence. Glenn

 March 19, 2004, 19:23 Re: Please help with flow around car modelling! #18 Neale Guest   Posts: n/a Sorry Tudor, I misintrepreted your question before. You can get a rough idea in CFX-Post of how well resolved your boundary layer is. In some slice planes take a look at how the velocity vectors vary from the car body to the free stream. Is there a nice profile or do you have like 2 vectors in most spots. That's all. You can look at yplus values as well but this is not so important if you are running SST. As Glenn also points out, if you have a nice grid you wont need transient uless you want to see the vortex shedding and how the drag varies in the transient due to that. Steady state is fine for getting the "averaged" value. If you are getting flat elements they you need to narrow in on the region where these are occuring and try putting in a bunch of mesh controls. You could also, as you point out, play with the number of inflation layers. 20 sounds like a lot. The bad elements can be the reason the residuals are hanging up so you should look at the end of the solver output file and find the node numbers of where the max residuals are located. Make a point locator in CFX-Post and see if that position corresponds to your bad grid at all, it probably will. Neale