# [ICEM] Simplified vehicle model (wheels intersection, density region)

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

 October 28, 2011, 14:13 Simplified vehicle model (wheels intersection, density region) #1 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 Hello, I won't be writing a lengthy post, instead I'll attach a .pdf that I've put together explaining where I'm stuck. Maybe it can help someone other beginner in the future. This post is mostly aimed at Simon, but please feel free to help if you can. OK, it seems the pdf is rather large, so I'll just be posting a link: http://www.mediafire.com/?8h6u4ipp598j77m Maybe just a few quick questions right off the bat.. Does a fillet need to be as large as I made it? Will it affect the rotating wall condition for the wheel? Or is the hole displayed in the pdf perfectly fine?

 October 30, 2011, 06:57 #4 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 Yes, turns out I'm an idiot again. It was enough to insert a sizing method and pick a single vertex at the rear of the car, then define sphere radius and max element size. I'm gonna try moving it around a bit more, try and optimize what I get, but here's the result for now: /edit I've been trying the Body of influence method because with the sphere I was limited to just the rear-most vertex on the car, but I'm not having much success with BoI method.. I might be doing something wrong, but when I add a body in the DesignModeler (I tried adding it as Frozen and Add Material) it results in a completely separate Geometry in mesher and then it meshes it as such, and screws up the domain. Pic: /edit 2 Got it! Here are the steps for anyone who cares (starting with DM): 1. Freeze the domain you already have (air for me). 2. Sketch your new rectangle or whatever. 3. Extrude by adding material (regular extrusion). 4. Freeze the new extrusion. 5. Boolean - Intersect - pick both bodies (air and new "wakebox" for me) - Preserve tool bodies (Yes) - Intersect type (Intersection of All bodies). 6. Under Parts/bodies you should now have 3: the whole air domain, the wakebox that follows the shape of the car and the original rectangular extrusion. Supress the original wakebox extrusion so you're just left with 2 bodies. 7. As Stuart said, in mesher right click Mesh - add Sizing - under Scoping method leave Geometry selection and pick the "air" (your main domain) as the Geometry selection - Type is Body of Influence - and under BoI pick the shaped wakebox (the only other geometry in the mesher) - define max element size and growth rate and you're done. Proof: P.S. Be careful when defining element size (I wen't for 15-20 mm at the begining and the mesh size jumped from ~2 mil elements to 8 mil). Last edited by scipy; October 30, 2011 at 09:17.

 October 30, 2011, 09:43 #6 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 It seems you were typing during my last edit In any case, I managed to solve the body of influence problem. Thank you for that article, I will go through it when I start the simulation run. Currently I'm trying to create a few more BoI's for the undertray and the wheel wells of the car and then I'm going to let it suffer through a calculation. For your last comment, you are right. This is my final project at college (I managed to talk my mentor into letting me do this instead of some usual 2D case they assign to 3rd year students) and the aim is to find Cd and Cl for 3 different car models which are all in the same "class", however the game is not mine but you can try the demo version for free if you visit www.lfs.net. The current problem with the GTR class of cars is that all 3 models have the same A and Cd (Cd is 0.2705 and A is 1.84 m^2) because it was easier for the developers to implement it like that when the Aero part of the sim was last updated, but it isn't really that realistic. I've already measured the frontal surface to be 2.131 m^2 and the last calculation suggested Cd was much lower than it should be - around 0.215 but some sort of correction factor will be used before game implementation. What I'm after is just comparsion of the 3 bodies and then we can increase all the Cd's to a realistic value, but still retaining the inherit differences between the 3 cars. Another thing that I'm after is the problem of slipstreaming/drafting as currently the car behind just loses huuuge downforce on the front end plus the effects of the draft are too drastic and can be felt from too far behind. As all of the cars just have a very simple front splitter the wake shouldn't really mean such a significant loss of (especially) front downforce. That's why I already split the car into named selections (because I was thinking about how do I get loses of lift/drag on separate surfaces like the undertray or front splitter) and now Fluent is calculating lift and drag forces for each individual component, which is what I needed in the first place. The other goal is to determine the behaviour of lift and drag based on ride height and rake angle of the car, but since this is only a game model and I removed all the complicated geometry like the front side fins, rear wing, mirrors etc, I'm not sure how realistic my results are going to be.. but again, I'm after a basic relationship and then the data can be corrected to get closer to realistic real life values for FIA GT cars or similar. As far as the books go, I've got Katz and JD Anderson but I am ordering McBeath on monday.. it'll take 20-40 days to get here, but it will be worth it. I've been reading his Aerobytes in Racecar Engineering and found out a lot of stuff there. I wish he'd write a tutorial for how he uses CFX, though. Last edited by scipy; October 30, 2011 at 10:00.

 October 30, 2011, 11:52 #7 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 Last update for now, as I'm going to run a simulation for the next oh.. 12-24 hours. I've managed to create two bodies of influence, one that captures the undertray and the wheel wells of the car, and the other is the "wakebox". At first I sized the elements to 10 mm in the undertray and 30 mm in the wakebox but this yielded a 14.9 million element mesh so I increased the sizes so that there's still a decent number of cells between the undertray and the road and also to capture the wake better than previously. Also, the element count is down to 5.7 million elements (previous simulation without any Sizing features had 2.7 million). Maybe people with more experience could comment on the size/position of the wakebox and the elements inside it. I know that ideally I should create several wakeboxes that would range in length, height, where they started on the car and element size, then run simulations on all these cases to determine how the convergence of results is behaving.. but maybe someone can suggest a decent guesstimate that would save me from all these cases. There is no rear wing and it's not an F1 car with a high and long wake, plus from the already posted screenshots of velocity plots on the symmetry plane suggest that the wakebox should be around 1-2 car lenghts behind the car. But since I don't quite know how to achieve a growth of elements from right behind the car moving futher and further back, I've limited it to the current size. One thought I had was maybe the wakebox should start at the joint between the roof and the rear windshield because the velocity seemed to have been changing there too and the previous mesh wasn't really all that dense there? Anyway, any suggestion is welcome at this stage, because whatever I decide on will be used for 30+ simulation runs later.

 October 30, 2011, 12:03 #8 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Cool, I have a few friends who are live for speed freaks, pretty cool game. Calculating losses from drafting and different pitch/ride heights is going to be fun.... I'm not so sure how easy it is to do with the workbench mesher, but scripting the simulation to run a bunch of cases would be the best way to do this. Moving your chassis shouldn't be too difficult, Ansys has a feature where you can specify parameters (ie ride height) and then have it simulate the flow at different values for that parameter. This feature used to be very tempromental and sometimes delete all the simulation data already created, but I have heard that it is now more stable, just be careful. As for testing for slipstreaming, you could have two cars and have a parameter for X displacement and Y displacement and then simulate across a range of different lengths. The front car should loose downforce off it's rear spoiler as well as the rear car loosing downforce off it's splitter and reducing drag. And if you really hated your social life, you could do what I'm doing and look at the changes in downforce and drag in cornering situations....

 October 30, 2011, 12:16 #9 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Unfortunatly theres no easy answer to how many elements you need, "as many as you can afford" is usually the general rule! What you have looks pretty good though. Solutions shouldn't take that long to run. Use the pressure based coupled solver, it is much faster than the segregated. Set the courant to 25 and then step it up by 50 every 100 iterations up to 200. Should solve in a few hours, not 12-24. Also if you are doing this at school, try getting access to a few computers at once. You can easily distribute the solution over 3 or 4 computers and it will solve even faster. As long as the computers are networked on (at least) gig ethernet, you will get pretty good speed up.

 October 31, 2011, 21:34 #11 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 Small update while I wait to be educated on solver setup.. I finished the simulation with a ~6 million element grid and wasn't really sure on the velocity over the rotating tires, so I repeated the simulation of just the tires to validate the case and I think it looks ok. The velocity on top of the tire is around +5 m/s and on the bottom it's -40 m/s (the air speed from inlet is -40 m/s in the X direction, or 40 m/s in the -X direction). Here are some screenshots which if I understood them correctly, confirm the results.

 November 1, 2011, 16:54 #12 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Thanks Stuart. I would raise your reputation (one of the little options in the bottom left) but it won't let me do it anymore than I already have. This thread will probably be one of those ones that thousands of people will look up for years, __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 November 2, 2011, 04:17 #13 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Haha, thanks Simon. I remember seeing your conversation with someone about meshing a Porsche ages ago and hoping that one day I too would be able to make sense of ICEM! Scipy: Glad you got your simulation to run, 5000 iterations is a long time though! I would be interested to know how you initialised your domain? That spike in residuals means that either your initialisation was way off (i.e. uniform flow at 40m/s rather than -40m/s) or that it was very close and the solvers first guess was off. I have this happen to me when using FMG initialisation because the first guess is usually more accurate than the solvers first iteration. Because all the residuals are scaled to the initalised value, you will never get a solution residuals plot that "looks" as good as with a poor initialisation even though the solution is better. Also, shouldn't the top of the wheel be moving at 40m/s forward? Are you sure the boundary condition is set correctly? Stu

November 2, 2011, 11:40
#14
Senior Member

Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 184
Rep Power: 8
Quote:
 Originally Posted by stuart23 Scipy: Glad you got your simulation to run, 5000 iterations is a long time though! I would be interested to know how you initialised your domain? That spike in residuals means that either your initialisation was way off (i.e. uniform flow at 40m/s rather than -40m/s) or that it was very close and the solvers first guess was off. I have this happen to me when using FMG initialisation because the first guess is usually more accurate than the solvers first iteration. Because all the residuals are scaled to the initalised value, you will never get a solution residuals plot that "looks" as good as with a poor initialisation even though the solution is better.
I used the Standard Initialization and Compute from velocity-inlet. As I've said, I'm keen to learn some proper Fluent solver setup because I'm using the most basic settings with the SIMPLE scheme and First order everything at the moment.

Quote:
 Originally Posted by stuart23 Also, shouldn't the top of the wheel be moving at 40m/s forward? Are you sure the boundary condition is set correctly? Stu
Let's clear something up first: if the wall is a no slip condition and I paint it with velocity contours, does that necessarily mean that the velocity of the air has to be the same as the wall rotation/translation velocity?

My understanding was that the top of the wheel has a tangent velocity component of 40 m/s forward (+X in this case) and that the airspeed coming on has -40 m/s (since it's in the -X direction) so those two should kind of cancel each other out somewhat and the result is around 5-7 m/s at that top blue contour. Ofcourse in this case there is no car, it was only the wheel. In the case with the whole car it is similar (-35 m/s at the contact patch, 1.7 m/s at the top of the wheel).

If I'm understanding something wrong, please do correct me. You can double check with the screenshots in the posts above where I defined the rotational axis for the wheels and the direction vector, too.

 November 2, 2011, 13:52 #15 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Just when you thought it was going to get easier, now that you mention it..... Yes you are sortof right regarding the wall velocity vectors. Fluent is a cell centered solver, and you are using first order upwind discretionalisation. This means that Fluent will calculate a value for your variables (velocity components, turbulent kinetic energy etc) and apply it to the entire cell. You can imagine that each cell has one discrete value and there is discontinuous steps between adjacent cells. You will therefore only see the velocity of the velocity at the centre of the bordering cell, and not the velocity of the wall. Where there is no shear (on your moving ground), the velocity is the same as the ground, but on the wheel,you have a large delta V, and therefore a difference between the flow velocity shown, and the flow velocity on the wall. If your mesh is fine enough on the boundary layer, the velocity at the centre of the first cell will be the same as the velocity of the wall. I kno that you are limited in cell count, soyou might want to consider using a turbulence model with wall functions so that Fluent will calculate the boundary layer using the law of the wall. Without a high mesh count or wall functions, you will not get accurate drag predictions. To measure the "accuracy" of the boundary layer calculations, we look at a variable called y+ AKA y plus. Y+ is a dimensionless distance that is calculated by multiplying your distance by the friction velocity and dividing by the kinematic viscosity of the fluid. The friction velocity is the square root of the shear stress of the fluid on the wall divided by the density of the fluid. When you plot y+ on a surface, it is the dimensionless distance between the wall and the first cell node (or centroid. Can't remember!). For wall functions, you need to have a y+ of about 30 to 100. Without wall functions you "should" have a y+ of about 1. Obviously not being able to read the speed of the wheel isn't that important, but the big difference does show that the mesh is not fine enough in these specific areas. Do you have prisms on the walls? If so what is the spacing?

 January 10, 2012, 13:48 #16 New Member   Nabil Z.A. Join Date: Jan 2012 Posts: 1 Rep Power: 0 Thanks for the step by step in creating the body of influence. Very useful!!

 April 1, 2012, 07:23 #17 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 Some video tutorials as promised in one of the earlier posts: http://www.youtube.com/user/eoescipy - Parts 1 through 3 for now.

August 28, 2012, 16:58
#18
New Member

ARUN V
Join Date: May 2012
Posts: 13
Rep Power: 6
Very usefull thread indeed...Thanks to Simon, stuart, scipy.
.
Has anyone of you tried including heat transfer in to the analysis
.
.I want to attach an exhaust pipe(thin wall tube with one end closed) along which heat transfer through convection occurs and hot exhaust gases escape into the surrounding air at high temperature and pressure
.
What i do is this:
1. Import the exhaust pipe in design modeller along with car
2. it is kept as a separate body(not included in Boolean subtraction)

3. In Fluent setup, the inside surface of the closed side(blue highlighted surface in above pics) is made as 'velocity inlet' boundary surface and temperature and pressure are specified.
4. I obtained the following result

ANYONE HAVE SUGGESTIONS TO THIS ??

Problems i am facing now are
1. heat transfer through the solid part of the exhaust pipe is not simulated(what should i do to mix steady state heat transfer and fluid flow)

(there is no temperature gradient accross the thickness of the pipe)
2. Though i specify pressure condition at inlet of exhaust pipe as 1000pa(gauge), this pressure is not shown inside pipe.
.
.
I think i have described my situation, please post if its not clear to you
Attached Images
 ex pipe1.jpg (21.3 KB, 4 views)
__________________
regards,
______________
ARUN V
Mechanical Engineerig student

 August 28, 2012, 17:31 #19 Senior Member     Alex Pasic Join Date: Aug 2011 Location: Croatia Posts: 184 Rep Power: 8 If the objective is to study the effects of the exhaust gases on the airflow around the car, then I'm guessing it'd be enough to have a full solid pipe (cylinder) that exists where it does on the car anyway - and then specify the end circular face as the velocity/mass inlet. Probably it's better to do it as a mass inlet so there's a conservation of mass and you can vary the temperature and pressure and everything stays the same.

 August 28, 2012, 19:06 #20 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 267 Rep Power: 17 Hi Arun, Do you want to set the boundary condition of the wall so that heat flux = 0? This can be done in the thermal tab of Fluent's boundary condition dialog. This way you will have a fully developed velocity profile at the exit, and a homogenous temperature profile. I know that this is not truly reflective of the profile of the actual exhaust of a car, but I do not think the extra effort will increase the accuracy of your simulation by much. Stu __________________ http://bc247.wordpress.com

 Tags car aerodynamics, density region, wheels

 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 Nina CFX 1 June 11, 2008 13:05 bohis FLUENT 0 April 14, 2008 03:08 bohis FLUENT 0 April 11, 2008 09:18 frederic felten Main CFD Forum 0 April 10, 2003 17:24 Ikhwan, Nur CFX 0 November 9, 2000 04:50

All times are GMT -4. The time now is 00:48.