# drag coefficient with k-eps model

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

 April 16, 2004, 05:38 drag coefficient with k-eps model #1 Mark Guest   Posts: n/a Hi, I'm calculating the 2D-flow over a NACA0015 profil with standard k-eps turbulence model. yplus values are between 20 and 100 along the chord. I'm am looking for an explanation for the following observation. Below stall angle the lift coefficient fits quite well to measurements. But the drag coefficient is far to high. At zero angle of attack some papers report a drag coefficent of approx. 0.0068. My calculated value is at 0.01. I think I understood why I can't expect too much beyond stall angle, but what might be the reason for that difference in drag? Best regards, Mark

 April 16, 2004, 09:03 Re: drag coefficient with k-eps model #2 ag Guest   Posts: n/a Are you running with wall functions? If not, then your value of y+ is much too large and your turbulence model is not modeling the boundary layer correctly.

 April 16, 2004, 10:39 Re: drag coefficient with k-eps model #3 Mark Guest   Posts: n/a Yes, I'm using the classical HighRe version with logarithmic wall functions. Regards, Mark

 April 16, 2004, 12:08 Re: drag coefficient with k-eps model #4 Dynamic Edge Guest   Posts: n/a Check your Cp at suction side. It might be too high and contribute a lot to the drag, esp. at high AOAs

 April 16, 2004, 16:30 Re: drag coefficient with k-eps model #5 CFD Rookie Guest   Posts: n/a Mark, what software are you using? Check the user manual on what is the range on y+ for KE turbulence model. Drag is always difficult to predict. There are lots of posts recently (either in main forum, CFX or in the fluent section) talking about this issue. I have been on this type of analysis for a few months now, and based on my experience, it is really really dificult to get computed drag as good as your computed lift. Y+ might be the main reason. Check you Cp vs X/C plot. Normally the pressure side curve will match up pretty well, the suction side Cp, especially on LE area, is toughest to match. If your Cp vs x/c has good match w/ experimental value, and your drag is still off, then it means your pressure drag is good, but the friction drag, which is a function of you turbulence model, y+ etc is the main reason it is off. By the way, what is your RE (chord)?

 April 19, 2004, 01:47 Re: drag coefficient with k-eps model #6 Mark Guest   Posts: n/a But shouldn't this error also affect the lift coefficient, which is quite well predicted in my calcuations?

 April 19, 2004, 01:48 Re: drag coefficient with k-eps model #7 Mark Guest   Posts: n/a

 April 19, 2004, 02:12 Re: drag coefficient with k-eps model #8 Mark Guest   Posts: n/a My Reynolds Number is 10e7. I think the problem must be connected with the friction drag, since even at an angle of attack of 0 degrees my drag coefficient is approx. 60% to large. 0.01 instead of 0.006. I just checked again the y+ values for 0 aoa. y+ rises fast from 0 at the stagnation point to 110 at 0.15 chord. Then it drops almost linearily to 70 at the trailing edge. Do you think that this values is to high and could be the reason for having 60% too high drag? Regards, Mark

 April 19, 2004, 09:55 Re: drag coefficient with k-eps model #9 CFD Rookie Guest   Posts: n/a Lift is affected by y+ too, but obviously not as signigicant as drag. Why don't you carry out a mesh dependency test. Refining or coarsening the mesh on the airfoil surface, thus gradually resulting in a lower or higher y+, then check your drag again. It is possible that with KE and standard (logarithmic) wall function the best drag result might not come from lower y+ values. Recall that y+ ranges between (approximately 35-350, this range depends on the code you are using). And the best drag result might come from any y+ values within the range. I know this is not an easy task at all. On the other hand, besides the issue of mesh, you also need to make sure your domain is adequately big enough. Mesh on the wake region (directly after the trailing edge) must be fine enough. Check your residuals monitor and try to locate the cell (or node or element) with the highest residual value (if the code allows the users to do just that), then try refining the mesh at that location. For this type of flow analysis, result based on residual level of 1e-3 and 1e-5 might be quite different. Note that I am not indicating 1e-5 is adequate. Maybe to get proper drag result, you need to go an even lower residual. This is what I can think of other than the issues of y+ and mesh. By the way, since we are on this subject, how close is your pitching moment result compared to the experimental values. Is Cm as good as Cl? Good luck. Let me know your latest progress.

 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 Ketut Utama Main CFD Forum 8 December 11, 2014 12:03 saii CFX 2 September 18, 2009 08:07 Amir FLUENT 0 March 5, 2009 11:28 Freeman Main CFD Forum 10 January 27, 2006 08:42 Avijit FLUENT 11 March 29, 2004 14:04

All times are GMT -4. The time now is 00:33.