# calculation of drag

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 7, 2006, 01:58 calculation of drag #1 CFD Guest   Posts: n/a For calculation of drag at subsonic, transonic, supersonic and hypersonic regions, what should be the combination of turbulence model and Yplus?

 March 7, 2006, 03:12 Re: calculation of drag #2 Razvan Guest   Posts: n/a The only thing that I am sure of is y+ MUST be around 1 to have better chance of predicting viscous drag, which is much harder to predict than shape drag. This is mostly influential in low subsonic regime. When velocity goes beyond M=1, shock drag appears and viscous drag importance diminishes, but it is still quite high. Anyway, my opinion is that when M>1.5 you have to be much more careful to the shockwave sharpness and wake grid resolution than y+ and turbulence model. About turbulence model, I cannot say that a particular model is clearly better...I would choose S-A in most cases, although RSM would be better, but is too computationally expensive. Razvan

 March 7, 2006, 03:21 Re: calculation of drag #3 CFD Guest   Posts: n/a What should be the wake grid resolution when M>1.5 ? If we r simulating flow over a cylinder at M > 1.5, what should be the wake grid resolution and grid size over the body? How we relate shockwave sharpness with grid resolution? Thanks

 March 7, 2006, 14:58 Re: calculation of drag #4 Freeman Guest   Posts: n/a y+ around 1? But this is when one is using enhanced wall functions, isn't it? While using the standard law of the wall y+ needs to be between 30 and 200... or am I mixing concepts here?

 March 7, 2006, 17:02 Re: calculation of drag #5 Razvan Guest   Posts: n/a Enhanced wall functions do not exist in Fluent. You are talking about EWT (Enhanced Wall Treatment). This is in fact a special implementation of wall functions which is intended to eliminate y+ constraint (it actually minimises the error when y+ is around 11, the worst possible value), but it is not so good, to say the truth. For best results, you need to go to y+=1. Classic wall functions must be used with y+>30 (but also y+<100 for satisfactory results). Most turbulence models are not valid in near-wall region so must use wall functions. S-A and RSM fall into this category. In Fluent, S-A uses EWT only. But you still have to be careful when using it, not to have 4 < y+ < 18!! Good luck, Razvan

 March 8, 2006, 01:26 Re: calculation of drag #6 Freeman Guest   Posts: n/a OK, thanks Razvan: I didn't know that SA only uses EWT! Regards, Freeman

 March 8, 2006, 02:06 Re: calculation of drag #7 CFD Guest   Posts: n/a May you plz inform us about the y+ limits for k-e & k-w models. Please inform me about relavent material from which I can get necessary information and importance about the y+ value limits for different turbulent models. Thanks

 March 8, 2006, 03:05 Re: calculation of drag #8 Razvan Guest   Posts: n/a k-e models are separated in 2 main categories: - high-Re-number models (standard k-e, RNGk-e, Realizable k-e, and other variants), which all need wall functions (standard&non-equilibrium wall functions work well with 30 < y+ < 100, with an upper validity limit of y+=300, and EWT which works best at y+=1); - low-Re-number models (there are many modifications to standard k-e model made by different researchers, in order to make k-e model valid all the way to the wall, but none of it is available through the GUI), accesible by scheme commands in Fluent. k-w models are actually 2: standard k-w and SST k-w. Both are low-Re-number models and to work properly need y+=1, and when you have this y+, you can select "transitional flows" option in GUI. But if you cannot provide a mesh with y+ around 1, you can use the modified versions of these models, which use wall functions, and you may have y+>30 meshes. These are default in Fluent. I hope you got it now, Razvan

 March 8, 2006, 06:35 Re: calculation of drag #9 CFD Guest   Posts: n/a What is the value of Re, below which we use low-Re-model?? In my case mach is 1.2, residuals have converge upto e-5,but Cd is still decreasing. Where should I suppose that solution has converge???

 March 9, 2006, 03:55 Re: calculation of drag #10 Razvan Guest   Posts: n/a Low-Re-number model = valid in B-L, down to the wall (Re number is decreasing in B-L because velocity is decreasing, so at the wall Re=0) High-Re-number model = valid only in bulk flow, not in B-L region, so it needs wall functions. In high velocity flows, Cd is a better convergence criterion, so trust it, not the residuals! Good luck, Razvan

 March 12, 2006, 23:44 Re: calculation of drag #11 CFD Guest   Posts: n/a In the flow (M = 1.4) over a projectile, which turbulent model should be use for the calculation of drag? As reynold is high around the projectile but low near the projectile surface.

 March 13, 2006, 03:09 Re: calculation of drag #12 Razvan Guest   Posts: n/a All this talk until now had a specific purpose: you to get at the point where you would be able to think for yourself, and not to always wait for somebody else to tell you what to do. If you're not there yet, no problem, I would not mind to do this. (This is may way of dealing with this, it is my creed, don't get offensed, please) I see you're a little bit confused with these "low-Re", "high-Re", bla-bla... Anyway, let me explain this to you: - at the begining of your calculation, YOU decide what grid spacing to use at the wall: y+ near 1 or near 30; - based on this you will then choose the turbulence model So, the rule is: GRID SPACING (Y+) DECIDES WHAT TURBULENCE MODEL TO USE (low-Re or high-Re), NOT THE FLOW!!! If we are talking about flow characteristics, then it is something else. This influences turbulence model choise by other means. For example: flow around an airfoil at low incidence is excelently solved using S-A model, but the same airfoil at high incidence, near stall must be solved using RSM, because of high adverse pressure gradients, strong detachement, etc., and probably using unsteady solver. Now, coming back to your problem, I'd say that for the start you should use S-A, with a y+=30. The actual grid spacing at the wall for M=1.2, and air at normal conditions, is somewhere around 0.1 mm. Use this value to build your initial grid. You will get a pretty strong detached shock, so you will need to adapt the grid using pressure gradients as the criteria. DO NOT adapt cylinder boundary to get the right y+, it is better to reconstruct the grid! This is very important, because adding cells by hanging-node adaption in the boundary-layer is very damaging for the precision of your calculation (this could affect separation point prediction and consequently drag prediction, so be careful). I think it is enough for now. One more think: send me a message from your e-mail adress, so I could send you a grid I built especially for your case. I would like you to build your own grid and then use my grid and compare the results. OK? Razvan

 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 PRASHANT GHADGE FLUENT 4 December 13, 2012 16:31 lc05 Main CFD Forum 2 November 1, 2010 08:50 abcdef123 Main CFD Forum 1 May 9, 2010 23:00 ArtyB Main CFD Forum 1 January 10, 2010 19:18 AB CD-adapco 6 November 15, 2004 05:41

All times are GMT -4. The time now is 08:13.

 Contact Us - CFD Online - Top