Turbulent flow around car body
Dear Friends,
I really need some help on this. Please do try helping me! :( I am simulating turbulent flow around car body. Can anyone please tell me how to set the parameters required for this simulation, such as the choice of solver, the best turbulent model to use, its parameters, time step size and so forth. Please do get back to me as soon as possible. Your help will be very much appreciated. Thanks ! 
Re: Turbulent flow around car body
Hi
Start with a steady 2D model with the segregated solver. The ke model would be ok. You only need a velocity inlet for the domain and a pressure outlet. Try having the upper boundary as high as possible with symmetry to avoid its enfluence on the flow. 
Re: Turbulent flow around car body
Hey Bro,
Thanks for your reply. Finally some one replied :) I am doing a 3d model for my thesis project and I am running out of time. Have you a done a 3d model before ? Do you have a case and data file that i could refer to ? Please get back to me asap. Once again thanks and looking forward to ur help 
Re: Turbulent flow around car body
Hi
I have done many 3D models, but not for a car. Regards 
Re: Turbulent flow around car body
Hi,
My PhD is on modeling airflow around a vehicle so what do you want to know? I can't send you any case files because my work is confidential and my meshes are of 10million cells+. The first thing you need to consider is what do you want to get from you CFD model? Just drag coefficients? There is so much you can do with the post processing tools but quite often you need to take steps in the model set up BEFORE you do any simulations. Please share with me what it is you want to get from fluent, how much resource do you have? Do you have access to parallel processing or are you just working on a desktop PC. I am away now for a few days but I can probably point you in the right direction. Best regards, Carl. 
Re: Turbulent flow around car body
Hey Carl,
Thanks for your encouraging offer of help. I am using the geometry of a car that is provided n the GAmbit tutorial guide. I am trying to predict the sources of prominent sound sources around a simplified sedan, using Lilley's acoustic source strength broadband noise model. In order to do so, I first need to calculate a steady or unsteady RANS solution. The thing is I do not know how to create a proper mesh for the car, what type of mesh to use, whether a y+ adaption is needed, and so forth. I am choosing to use the k epsilon model for this flow proble. The flow is turbulent. I do not know what to set for the under relaxation factors, the coefficient values for the k epsilon model and so forth. I am really hoping that you will be able to point me in the right direction, as I am very short of time to do trial and error tests. Looking forward to your help and guidance. Thanks again Regards, Arjun 
Re: Turbulent flow around car body
By the way
I do not have access to parallel processing and I am using a desktop. Its an HP wokstation xw 4400. So i think it should be suffiecient. Thanks looking forward to your favorable help :) Regards, Arjun 
Re: Turbulent flow around car body
Hi Arjun,
Unfortunateley I know nothing about aeroaccoustics so I can only help with the steady RANS solution. So here goes: Essentially what you want from Gambit is a shape of the air volume surrounding the car. This then needs to be meshed and the boundary conditions set. If you have a gambit model of the air shape then that is a good start. Ideally you want the air volume to be pretty large, I tend to make sure that the frontal area of the vehicle being modelled is no greater than 5% of the domian, otherwise you get large blockage effects. Also, the domian length needs to be sufficient to capture the wake. I tend to place the inlet about 5 car lengths upstream of the car and the outlet up to 20 car lengths downstream. Now if you are using a desktop PC for this then you may struggle and so it may be better to downscale slightly. Remember though, you can grade the mesh so that it is extremely coarse on the domain outer boundaries and fine close to the vehicle  this limits the cell count. There are no guidlines to follow with this because you are working with certain resources. I wouldn't recommend using more than 650,000 cells with a single PC. I'm lucky enough to use 50 processors on 10 million+ cells but thats possible at universities. Meshing: Where do I start!?! It takes lots of trial and error and practice to get it right. You obviously dont have time to look at everything but if you can, use as many structured cells as possible. I would decompose you solution domain by splitting it around the car with faces. That way you can use nice ordered blocks of Hex cells with line controls to grade the mesh density. Use fine spacing close to the car and coarse far away. However, this will take weeks to get right. If that is too long just use an unstructured mesh. Put a coarse face mesh on the outer boundaries and a fine one on the car. Then use a volume mesh to fill in the space with cells. Check your mesh quality, you want the equiangle skew to be less than 0.9 if possible else you will encounter problems trying to solve later. Set the inlet boundary condition (BC) as a velocity inlet. Define the floor as a separate wall (you will need to give this a translational velocity matching the velocity on the inlet in fluent later). Set the outlet as a pressure outlet and sett the domain sides and roof as symmetry BC's. Once you have set the continum also (air), you can export a 3d mesh  this may take a while to write so be patient. Solving: Once you have read you mesh file into fluent, click on grid>reorder  this saves so much time in simulations by reordering the nodes. Then scale your grid, grid>scale  make sure you get this right! Set you boundary conditions i.e. inlet velocity and the ground plane velocity. It may be worth lowering the residual monitors, they are set at 0.001 but drop that to 0.0001 to make sure you get convergence later. Set your turbulence model define>viscous. I would use the standard kepsilon at first, this is easy to converge and you can use the result from this to initialize another turbulence model. Initialize the solution at this point and watch the residuals come down. When you have you solution, write the case and data file  you don't want to loose this! Next I would change the turbulence model to either the realizable kepsilon or the Spallart Almaras model  they are both used for vehicle aerodynamics. Also change the model to 2nd order, solution>controls, this is because the defualt setting are 1st order. 1st order simulations converge easily but they are not as accurate, that why it is better to start with first order and then use that data set to start a second order model off. Next, read in your first order data set and click iterate WITHOUT initialising the solution  the first data set already does this for you. At first there will be a jump in the residuals but they WILL come down, it may take a few thousand for this to happen. And that is just about it. You will have a steady solution to you problem. OBviously there are many subtleties to what I have just described but unfortunatley I can't teach you that  it comes with experience. So if I were you, give the above a try and it you are struggling, ask me questions if you want but it is up to you to do this. Good luck with the modelling, all the best. Carlos. 
Re: Turbulent flow around car body
Dear Carlos,
I cannot thank you enough for the detailed explanation you have provided. The sedan model I am using is the same as the one used in the gambit tutorial no 5. I will start working on the mesh over the weekend. There is a way where i can check the quality of my mesh in FLUENT as well, i think its called grid adaptation if im not mistaken. How do i apply this grid adaptation to improve the quality of the initial mesh ive made. The sedan does not have wheels and it is floating slightly ablove the floor. Any improvements I should make ? Your guidance and advice is my only compass, as I have no one else to refer regarding this matter. Thank you and looking forward to your reply 
Re: Turbulent flow around car body
Hi Arjun,
I am not familiar with the fluent tutorials but the sedan you mention should be a good basis. It is probably best that your car is floating above the ground because there are all kinds of problems with the mesh near tyre contact patches touching the ground. You may want to add a series of half cylinders to the body of the car to represent wheels if you can do this. The easy option would then to lift the car off the ground so that the wheels are maybe 10cm off the ground  there needs to be enough of a gap for some cells to fit. If you are feeling brave however, place a plane about 5cm up from the bottom of the cylinder wheels and cut these bottom bits off. Then lower the car so that these new 'flat' bottoms are in the same plane as the ground. At this point just be careful with meshing in this area because it is easy to have distorted cells in these areas. Other than this I wouldn't make any other improvements, they are unlikely to benefit you much if time is of the essence. You can check the quality of your mesh in Fluent but not with adaption. If you want to do this you can do a histogram in one of the display commands  cant remember which one. However, if you check the mesh quality and it is poor then you have to go back to Gambit to change it again! So it makes sense to get it right in Gambit in the first place. Grid adaption cannot simply change the grid straight away. The idea behind it is that first you get a solution using the original mesh. Once you have this solution, thats when the grid can literally be distorted/adapted to match the solution better, before a new solve on this adapted grid is done. For example if the flow accelerates over the Sedan bonnet/hood and the change in speed is high, you can adapt the grid with respect to velocity. Fluent will then add more cells in that region to better resolve the airflow, because the velocity gradients are high. What I would say though is that grid adaption can take a while to get used to  I have very little experience in this area. I rely on taking more time in creating good grids in the first place. I suggest you do the same, otherwise you will never finish your project! Glad to be of help, good luck... Carlos. 
Re: Turbulent flow around car body
Dear Carlos,
Hope you are keeping up well. Ive finally worked out the car, mesh and boundary conditions! :D The total number of cells came up to 315000. I had first created about 712000 or so cells but realised that it would probably be a little bit too heavy for the current resources i have to process the iterations. I created 315000 as a first base, as i know fluent will increase the no of meshes or cells using grid adaptation. I was wondering if i could send you the mesh file for some feedbacks on improvements that can be made. I was also wondering if you could guide me on what to do next. Thank you in advance. Looking forward to your favorable reply. Best regards, Arjun 
Re: Turbulent flow around car body
Hi Arjun,
I can have a quick look at the mesh for you. Send it to mecarlg@yahoo.co.uk and I'll check it out. Once the mesh file is written then you're well on your way. Carlos. 
Re: Turbulent flow around car body
Dear AAA,
I am performing a tubulent flow around a simplified sedan. I am using the standard ke model. I have a few questions and hope you could help me clarify them. Do i use a steady, (if so why) or an unsteady model (if so why). What values do you think is best to set for the turbulent parameters in the boundary conditions? I heard that we need to supply a value for k and e. in which step of the steup do i do this and what is the formula to do so ? 
Re: Turbulent flow around car body
Hi
Choosing betwen steady and unsteady simulations really depends on what you are trying to find. Performing a steady simulation gives the average values of the variables (T, v, etc.), while an unsteady one offers timedependent values. The BCs depend on your case, such as the velocity of the car and wheather there is a car driving in front of yours causing turbulence and effecting your car. I'd say the easiest way is to specify a turbulence intensity and length scale, which can be obtained from the literature in this field (Try Google Scholar w/ CFD, car, turbulence). Again, I'm not an expert in the automobile field, so try to find an article that discusses the BCs of the domain. Regards Regards 
Hi Arjun, can you tell me where to download the sedan file for tutorial 5 or do you still keep the file? Can you send it to me? Many thanks! jkkt87@hotmail.com

All times are GMT 4. The time now is 22:06. 