
[Sponsors] 
March 8, 2004, 20:26 
Please help with flow around car modelling!

#1 
Guest
Posts: n/a

Hi All, I'm new to CFX so I have some dumb questions  sorry. I'm using CFX for automotive project  trying to design a good aero package for race car. I tryed my first solution and already have some problems: First I saved SolidWorks file as IGES and imported it in Build. I choused mm's for new database as I was told that this is the way to go with IGES files.
Solid created nicely. I went on to create the mesh – choused 5 for max edge length (mesh parameter), created Mesh Control and choused 1.5. Inflation parameter 5. For inflation boundary I choused model and flour as most important areas. Proximity set to 4. Created 3D and 2Dregions Than I made a GTM file and went to Pre. Domain, than Car body itself – no slip, domain top, side and bottom walls – added to region and free slip. Front wall – Inlet: subsonic, normal speed 44.44 m^1, Turbulence medium 5%. Outlet: subsonic, Average static pressure, 0 Pa. Symmetry plane – symmetry. Domain models: Air ideal gas, ref. pressure 1e05 Pa, no buoyant and stationary. Fluid models: Isothermal, 25C, SST, rest as default. Steady state Solver control: High resolution, Physical timescale 1s, RMS 0.0001, Dynamic control on Body Forces – averaging type Volume –weighted. Went to solver and started run. Solver showed that mesh has Total Number of Nodes = 176886 Total Number of Elements = 670227 Total Number of Tetrahedrons = 519362 Total Number of Prisms = 150865 Total Number of Faces = 47961 It solved with no probs and target convergence was achieved. Than I went to Post and got very strange numbers Lift 1.64Nm and drag 0.24Nm ….. that looked VERY wrong . This was a model of car with full length tunnel and pressure plot showed very good pressure drop under tunnel also in my wildest dreams I can't expect 0.24Nm of drag! Also when I created a point to attach a streamline it all got strange – to fit in domain (15m long) I had to choose 0,02 0.001 0.15 ! I started to wonder what units is it…. Than I went back to builder and checked again geometry units – it was mm's. Than I tried to create a point with 1000 1000 1000 coordinates – could not see it. So to get within domain I had to make 50 50 50 ! So now I have a feeling that some how my model shrunk to very small thing…. I have to say here that I have limited time access to program – 2 hours a day – no more. So it's hard to study manual really carefully. Any advise will be highly appreciated. If anybody has experience with modeling flow around car and correlated it to wind tunnel results please give me some advise on boundary conditions etc. Thank you Ted Sorry for such a long post. 

March 9, 2004, 08:11 
Re: Please help with flow around car modelling!

#2 
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, 10:43 
Re: Please help with flow around car modelling!

#3 
Guest
Posts: n/a

I reruned the model with coarse mesh (221000 nodes)and when in SFXCPost 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, 18:57 
Re: Please help with flow around car modelling!

#4 
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, 08:05 
Re: Please help with flow around car modelling!

#5 
Guest
Posts: n/a

Hi Glenn, Thanks a lot for your help. While I found some resent SAE papers referring to Ahmed body: 2004011308, 2004010442, 2002013349, 2001012742, 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 steadystate, is it proper way? 4) What is proper convergence target? 1e4? 1e6? I've heard from one person that decent results can be had with 1e3… 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 CFXPost 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, 18:01 
Re: Please help with flow around car modelling!

#6 
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://wwwwaterloo.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://wwwwaterloo.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) CFXPost 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, 22:07 
Re: Please help with flow around car modelling!

#7 
Guest
Posts: n/a

Answers to your questions:
1. 1/3 is pretty good. If you experience robustness problems then 1/41/5 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. 1.0e3 MAX is good for ballpark solutions and 1.0E4 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 510 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 nonconvergence 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://wwwwaterloo.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, 16:44 
Re: Please help with flow around car modelling!

#8 
Guest
Posts: n/a

Glen, Neale, You guys ROCK! Your help is highly appreciated. As far as I understood with inlet turbulence model I can simulate my car running in "clean" or disturbed air. How ever if inlet is far from model than it will "dissolve" before reaching model and it would not solve – hope that I got it right. In CFX tutorial 5, using Ahmed body, Author suggests to use for inlet b/conditions intensity and length scale option for turbulence with 0.05 value for fractional intensity and 0.1m for Eddy length scale. Should I consider this as "clean" air stream? As mentioned in previous posts I used 5%. Here another question arises – if I want to simulate my car fallowing a competitor closely (inlet as close as virtual competitor simulated)– what turbulence option I should use? This condition is known to cause drop in both drag and lift allowing faster straight line speed but possible problems in fast sweeping corners. One very dumb question – how many prism layers I have in boundary layer when setting inflation parameter?
I did comparative runs with different convergence target. Here's results: 1e3 1e4 1e5 L = 1013.17N L = 1222.83N L= 1304.7 D = 87N D = 108.6N D = 114 I guess this is because of the nature of my model. How can I upload a file (text or image) to this forum? My model is not a car yet but a blunt body with horizontal upper surface and inverted airfoil shape lower surface. Side "skirts" 1.5" from ground and 1.38" from "tunnel" lowest part. 106" long and 58" wide. Looking at model in CFXPost big part (may be main part) of downforce is caused by air leaking from sides into lower pressure area after tunnel upsweep. This air creating vortex – very fast as they get under car. This causes low pressure zones. It also helps the flow to stay attached to tunnel surface – in the longitudinal middle of tunnel where vortexes don't influence flow seem to separate about 18" from end of tunnel. Closer to sides where vortexes exist flow stays attached. I suspect that because of this vortexes finer convergence gives different numbers. If this is the case I guess that I just have to keep raising the bar till results stabilize. May be I'm wrong and this difference in results indicates some problem in the way I set the simulation. As model is symmetric I run a half only but it's seems to be wrong as those vortexes are pointing towards car centerline. So If I run it as full model they should interact probably canceling each other. I'd like to kindly ask you to take a look at part of my output file. May be there's some obvious mistakes? I know that this information is by far not enough but I can upload needed files to FTP if necessary. I'll have to ask about license number to be able to log into CFX community forum. As I told you I don't own the program but friend of my kindly giving me some "machine time" – I don't know what his boss will say about giving me license number to log in… Once again I want to say THANK YOU for your help. Ted SIMULATION TYPE : Option = Steady State END DOMAIN : JT2 Coord Frame = Coord 0 Domain Type = Fluid Fluids List = Air Ideal Gas Location = JT1 DOMAIN MODELS : BUOYANCY MODEL : Option = Non Buoyant END DOMAIN MOTION : Option = Stationary END REFERENCE PRESSURE : Reference Pressure = 1e05 [Pa] END END FLUID MODELS : COMBUSTION MODEL : Option = None END HEAT TRANSFER MODEL : Fluid Temperature = 288 [K] Option = Isothermal END THERMAL RADIATION MODEL : Option = None END TURBULENCE MODEL : Option = SST END TURBULENT WALL FUNCTIONS : Option = Automatic END END BOUNDARY : Inlet Boundary Type = INLET Location = Inlet BOUNDARY CONDITIONS : FLOW REGIME : Option = Subsonic END MASS AND MOMENTUM : Normal Speed = 44.44 [m s^1] Option = Normal Speed END TURBULENCE : Option = Medium Intensity and Eddy Viscosity Ratio END END END BOUNDARY : Outlet Boundary Type = OUTLET Location = Outlet BOUNDARY CONDITIONS : FLOW REGIME : Option = Subsonic END MASS AND MOMENTUM : Option = Average Static Pressure Relative Pressure = 0 [Pa] END END END BOUNDARY : FreeWalls Boundary Type = WALL Location = FreeWalls BOUNDARY CONDITIONS : WALL INFLUENCE ON FLOW : Option = Free Slip END END END BOUNDARY : SimP Boundary Type = SYMMETRY Location = SimP END BOUNDARY : BodyJT2 Boundary Type = WALL Location = BodyJT1 BOUNDARY CONDITIONS : WALL INFLUENCE ON FLOW : Option = No Slip END END END END INITIALISATION : Option = Automatic INITIAL CONDITIONS : Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS : Option = Automatic with Value U = 44.44 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END EPSILON : Option = Automatic END K : Option = Automatic END STATIC PRESSURE : Option = Automatic END END END SOLVER CONTROL : ADVECTION SCHEME : Option = High Resolution END BODY FORCES : Body Force Averaging Type = VolumeWeighted END CONVERGENCE CONTROL : Maximum Number of Iterations = 100 Physical Timescale = 0.125 [s] Timescale Control = Physical Timescale END CONVERGENCE CRITERIA : Residual Target = 1e5 Residual Type = RMS END DYNAMIC MODEL CONTROL : Global Dynamic Model Control = Yes Data Type Kwords Words/Node Words/Elem Kbytes Bytes/Node Real 121256.0 331.07 90.85 473656.1 1324.29 Integer 48686.4 132.93 36.48 190181.2 531.73 Character 1450.5 3.96 1.09 1416.5 3.96 Logical 40.0 0.11 0.03 156.2 0.44 Double 908.0 2.48 0.68 7093.8 19.83 ++  Total Number of Nodes, Elements, and Faces  ++ Domain Name : JT2 Total Number of Nodes = 366251 Total Number of Elements = 1334664 Total Number of Tetrahedrons = 979224 Total Number of Prisms = 355440 Total Number of Faces = 84272 Execution terminating: all RMS residual AND global imbalance are below their target criteria. ================================================== ==================== Boundary Flow and Total Source Term Summary ================================================== ==================== ++  UMom  ++ Boundary : BodyJT2 6.2704E+01 Boundary : FreeWalls 8.3726E01 Boundary : Inlet 3.1629E05 Boundary : Outlet 2.6912E+02 Boundary : SimP 2.0535E+02  Domain Imbalance : 1.9046E+00 Domain Imbalance, in %: 0.0202 % ++  VMom  ++ Boundary : BodyJT2 1.3047E+03 Boundary : FreeWalls 1.2674E+03 Boundary : Inlet 5.1498E06 Boundary : Outlet 3.7485E+01  Domain Imbalance : 1.7258E01 Domain Imbalance, in %: 0.0018 % ++  WMom  ++ Boundary : BodyJT2 1.1404E+02 Boundary : FreeWalls 3.2405E04 Boundary : Inlet 9.4220E+03 Boundary : Outlet 9.3072E+03  Domain Imbalance : 7.5684E01 Domain Imbalance, in %: 0.0080 % ++  PMass  ++ Boundary : Inlet 2.0814E+02 Boundary : Outlet 2.0814E+02  Domain Imbalance : 2.0294E03 Domain Imbalance, in %: 0.0010 % ================================================== ==================== Wall Force and Moment Summary ================================================== ==================== Note: Pressure integrals exclude the reference pressure. To include it, set the expert parameter 'include pref in forces = t'. ++  Pressure Force On Walls  ++ XComp. YComp. ZComp. BodyJT2 6.3521E+01 1.3049E+03 9.5062E+01 FreeWalls 8.3525E01 1.2635E+03 0.0000E+00 ++  Viscous Force On Walls  ++ XComp. YComp. ZComp. BodyJT2 8.1729E01 1.9257E01 1.8977E+01 FreeWalls 1.9481E03 3.9170E+00 3.2405E04 ++  Pressure Moment On Walls  ++ XComp. YComp. ZComp. BodyJT2 7.6300E+02 1.7431E+02 5.4323E+02 FreeWalls 6.2944E+02 1.0596E+03 5.0946E+02 ++  Viscous Moment On Walls  ++ XComp. YComp. ZComp. BodyJT2 2.1958E+00 7.2550E+00 1.5856E01 FreeWalls 7.8970E+00 8.1475E03 5.5444E01 ++  Locations of Maximum Residuals  ++  Equation  Node #  X  Y  Z  ++  UMom  12249  7.281E01  0.000E+00 5.989E01   VMom  12249  7.281E01  0.000E+00 5.989E01   WMom  36418  0.000E+00  5.576E02 5.842E+00   PMass  74048  0.000E+00  1.184E+00 5.842E+00   KTurbKE  125541  7.188E01 2.557E03 6.173E01   OTurbFreq  12021  7.197E01  0.000E+00 6.168E01  ++ ++  Peak Values of Residuals  ++  Equation  Loop #  Peak Residual  Final Residual  ++  UMom  1  5.29802E05  6.75326E06   VMom  1  2.63665E05  2.38653E06   WMom  1  9.03116E05  9.93734E06   PMass  1  1.31405E05  1.38309E06   KTurbKE  1  1.64213E04  9.63895E06   OTurbFreq  2  1.92829E04  1.50320E05  ++ ++  False Transient Information  ++  Equation  Type  Elapsed PseudoTime  ++  UMom  Physical  5.99540E+00   VMom  Physical  5.99540E+00   WMom  Physical  5.99540E+00   PMass  Physical  5.99540E+00   KTurbKE  Physical  5.99540E+00   OTurbFreq  Physical  5.99540E+00  ++ ++  Average Scale Information  ++ Domain Name : JT2 Global Length = 3.3930E+00 Maximum Extent = 1.0160E+01 Density = 1.2050E+00 Dynamic Viscosity = 1.7900E05 Velocity = 4.6116E+01 Advection Time = 7.3575E02 Reynolds Number = 1.0534E+07 Speed of Sound = 3.4057E+02 Mach Number = 1.3541E01 

March 11, 2004, 17:13 
Re: Please help with flow around car modelling!

#9 
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 1e5 (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, 17:36 
Re: Please help with flow around car modelling!

#10 
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, 08:21 
Re: Please help with flow around car modelling!

#11 
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, 17:23 
Re: Please help with flow around car modelling!

#12 
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, 01:37 
Re: Please help with flow around car modelling!

#13 
Guest
Posts: n/a

Tudor,
Your physics setup looks fine. I would just turn off the body force averaging though, that does not matter for your case. You will know how many inflation layers you have because you should have set this when you created the mesh in CFXBuild. You can control these settings in Build using Set>Inflation Parameters on the meshing panel. You could also load the grid into CFXPost, throw a slice plane across your body and just count how many prisms you see before the mesh turns into tetrahedrons. If you don't have at least 510 prism layers in the boundary layer you will not get good drag predictions. Lift may be OK, but drag will not be. As for inlet BCs, my comment about turbulence dying out only applies if your inlet BC is far upstream of the car. say 50 car lengths or something like that. This does not sound like it is your case. Probably 5% and default length scale are just fine for your turbulence conditions. Even if you are trying to simulate a car just in front I would not go higher than 10% or so. If you have converged to 1.0 E5 RMS residuals you should simply check how far the MAX residuals have come in. In some cases, if the flow is not hung up on some bad grid (as described by Glenn) the MAX residual will follow RMS by an order of magnitude (1.0E4 in your case). Just right click in the solver manager and select "switch residual mode" to check where the MAX values are at. If these are 1.0E3 or below you can probably be pretty sure you have a reasonable solution on your current grid. You could try, if you want, to get it to 1.0E4 MAX but this may only be possible if you have enough grid resolving all "tough" regions of your flow. Since your flow is basically incompressible, one other thing you might try is running a constant blend factor advection model instead of highresolution. Just switch this on the solver control panel and set a value of 1.0. This will run a bit faster and you may get a better result than with highres. Caveat is that you may encounter some robustness/convergence difficulty (eg: not being able to get MAX residuals down or something like that), which may require grid refinement. Make sure you plot the force on the car in the solver monitor as well, to see if it is changing. If it is not, or is oscillating around some average value, then you can assume that the solution is complete. Neale 

March 17, 2004, 16:15 
Re: Please help with flow around car modelling!

#14 
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 1E04 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 1E4.8 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, 17:36 
Re: Please help with flow around car modelling!

#15 
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, 18:10 
Re: Please help with flow around car modelling!

#16 
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, 17:44 
Re: Please help with flow around car modelling!

#17 
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, 20:23 
Re: Please help with flow around car modelling!

#18 
Guest
Posts: n/a

Sorry Tudor, I misintrepreted your question before.
You can get a rough idea in CFXPost 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 CFXPost and see if that position corresponds to your bad grid at all, it probably will. Neale 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Finding volume flow rate through a car  wh88  FLUENT  0  September 23, 2011 14:12 
Flow on a car!  John222  CFX  3  January 24, 2011 19:43 
ask help on valve flow simulation(3D modelling)  Anna  FLUENT  0  July 18, 2003 17:39 
Compressible Flow Modelling?  yeo  FLUENT  4  March 7, 2003 08:08 
Inviscid Drag at subsonic, subcritical Mach #  Axel Rohde  Main CFD Forum  1  November 19, 2001 13:19 