[bennn]

Hey everyone, first question for me here.

I'm running simulation of Darrieus turbine, 2 blades rotating around an axis perpendicular to the flow. We want to compare turbulent and transition models, so Velocity profile would be very useful...

however I can't find a way to do that easily... I've been through all the tutorials and this forum, I thought there would be an easy way of doing that.

the thing is since my foil is rotating around an axis which is 10 chord away from its centroid, its position keeps changing, so i can't define lines.

The closest I found is to make a plane just around the foil, rotate it with the formula omega*t, then export the BC profile, and the file I get is very hard to use...

If it's a silly one i'm really sorry, I'm pretty much new to CFX, and post is quite difficult to use I reckon...

thanks

ben

[ghorrocks]

Why don't you put the turbine in a rotating frame of reference, connect it to a stationary frame of reference with a GGI and then you will have a simple planar and stationary inlet and outlet surfaces.

post is quite difficult to use I reckon

? I can't see how post processing could be any easier than with CFD-Post. I have no idea what you are getting at here.

[bennn]

thank you very much for your help !

I already have a rotating frame. My domain is made of a rotor : a ring with the foils which rotates ; and a stator : a rectangle domain and a central circle domain. Connection is made with GGI.

The thing is i can't find a way to access the rotating coordinate frame... as i said i went through the whole help and this forum...

Not sure if I explained it right, but what I want to plot is the velocity profile in the AIRFOIL boundary layer. something using the normal to wall boundary would be perfect. I found polyline has an associated "normal" variable, but I can't find a way to use it.

And concerning the easiness of use, if what you say is right then I must really be stupid... With all the due respect, I think CFX is an awesome solver, but all the environment around it can be improved. I have at least 10 examples where the program was obviously the cause, i'd be glad to talk about it. With the use of command editor I guess it has no limit, but I couldn't find anywhere with beginner examples or tutorials...

then again, i really don't want to be disrespectful, you're the man here...

[ghorrocks]

i can't find a way to access the rotating coordinate frame

But the "Velocity" variable field is in the rotating coordinate frame. The variable "Velocity in stationary frame" is in the stationary frame. You should be able to plot boundary layers using the Velocity variable.

but all the environment around it can be improved

Agreed, it is far from perfect and other CFD solvers have a superior user interface in many respects.

but I couldn't find anywhere with beginner examples or tutorials.

This is a major failing of CFX. It is very difficult to find examples for the more advanced functions. These examples exist, you just need to talk to CFX support to get them, or do one of their training courses.

i really don't want to be disrespectful

No offense taken, I have no allegiance to CFX and as soon as a better CFD code comes along I will switch to it.

[bennn]

Yes I kinda understood the difference between velocities. I was able to plot the velocity field as a vector field, which enables me to have a look at how the fluid is moving in boundary layer.

The thing is I want to have precise velocity profile, that is graph that plots velocity as a function of normal distance from the solid boundary, you know, the classical results one can see in every book.... like that http://furtech.typepad.com/.a/6a00d8...9c26970c-800wi

The vector field is awesome, but you can't really get anything quantitative with it....

thanks again. I'll try to contact cfx people, but I've done it once so far with no success...

why not start a sticky thread with examples of CEL routines ???

ben

[ghorrocks]

Can't you simply draw a line normal to the surface - if you don't know the normal vector just draw a line and adjust until approximately normal, then either export the velocity along the line or draw velocity vectors along the line to visually see the boundary layer?

[bennn]

Yeah I've done that already, the thing is I'd like to get at least 10 profiles along the chord, and the airfoil is moving around a central axis which is ten chord away, pretty much like that : http://www.windturbine-analysis.netf...pathvector.gif


My problem here is to find a solution so that the line moves with the rotating domain (a ring).

I noticed there's a variable called "boundary normal on polyline", which sounds very good since my polyline is drawn around the airfoil surface.... but I couldn't find any information about that variable...

And if you don't mind giving me your opinion about something else, we're having interrogations about the timestep as well... you said the RMS courant shouldn't go beyond 10-20 in a previous post, right now I tried 3, 7, 15 and 20. 3 and 7 give similar results when wake has been convected far enough, I'm waiting for the 2 other to finish being solved. 7 looks pretty good, but for a complete calculation it's 1 or 2 months of computation...

What is your experience with comparing different solutions at different courant number ? Can the result become REALLY different, or can we speed up the timesteps and find results with like 10% difference at most ? The only info I got from the solver's Help is that it's unconditionnaly stable (implicit), but that transient LES needs low enough timesteps.

Thanks a lot for your help. It's truly appreciated.

ben

[ghorrocks]

My problem here is to find a solution so that the line moves with the rotating domain (a ring).

Then setup the lines, and with a session file move them as a function of how far the domain has rotated.

Your question about time step convergence sound vague. Are you just looking at the results and seeing what they look like or are you plotting an important variable versus timestep size? A true timestep convergence study is quite mathematical - see http://journaltool.asme.org/Template...umAccuracy.pdf, or even better look at the seminal text in the field of CFD accuracy "Computational Fluid Dynamics" by Roache.

Also, I don't in general recommend courant number time stepping. I recommend adaptive timestepping, homing in on 3-5 coeff loops per iteration. This generally gives you timesteps which are pretty close to time step converged, but you will need to check this for your case.

Are you using second order timestepping? Timestep convergence is much easier in second order, that is why you use it.

[bennn]

ok thanks I'll try that.

I'm plotting the force applied to an airfoil vs the timestep.... Yeah it was vague I'm sorry, I wanted to get easy answer to dodge the good ol' timestep study, but I guess I'll have to do it.

But here is something more interesting, I tried 3,8 and 15 as a courant number. 3 and 8 are equal, 15 is a bit different. Now I'm trying to simulate the same kind of system with a radius twice as large. hence the velocity gets twice as large, and courant gets roughly twice as large.

then is it definitely ok to say that the RMS courant can be kept the same as the trial runs, and we'd get good results confidently ?

thanks

[ghorrocks]

That's up to you to judge. If the flow is in a similar regime then probably yes. If the flow changes regime (ie transition points move a lot, compressible effects gain importance, whatever) then no.

But as I said I recommend doing 3-5 coeff loops per iteration and you let the adaptive timestepping find the timestep size each time.