The mesh at hub does not look good.

Do you have 10-12 points in boundary layer?

Which turbulence model you are using?

use newer version of fluent which is equipped with hybrid wall function for SST model.

https://dl.dropbox.com/u/35161486/sudden.PNG

this sudden change in the element height should raise some awarness. i usually go by a ratio of 1.2 up to 1.5. yours is more than triple.
I don't know what the others members think about it...

Ali from where you got this pic?

bollonga's post in the attached pictures. right button click and get the image url

Well, I'm running now the same case for U=10m/s. Reverse back-flow has disappeared but force and moment coefficient remain so low.
15R downwind is not long enough?

I have 15 layers near the wall,starting at 4e-6 m aprox so I have y+<1. How thick is the boundary layer supposed to be?
By now I'm running the laminar case, I'll use k-omega SST later on.
Which fluent version? 14.0? How does hybrid wall function works?

You're right. Trying to reduce the element number I've left size changes like this. I'm gonna fix that. But do you think this can be the reason for such distorted valued?

Hi everyone, I've run the cases with increased windspeed (10 and 15 m/s) keeping the same angle of attack. The mesh is the same and it's still single precision. As I said before, reverse flow has disappeared. However, torque is still too low. Cm=0.004 aprox. It yields a power at least 5 times lower than the experimental data.

I'm now running the same cases for windspeeds of 5, 10 and 15 m/s with double precision. At least my PC is not running out of memory with this mesh.

Once I have finished I will increase mesh density around the blade and try again, but I don't know if this will be enough to increase the torque to a value near the experimental value. I guess I will need to test some other angles of attack, now I'm using 12º.

I have a new question about rotating meshes... what's the difference between "rotating reference frame" and "rotating mesh" in the "cell zone condition" tab?

Double precision rise the same results as single precision. But I made a mistake in the power calculation, it's giving aproximately 10 times less than the experimental data.:(

I've also tried to reduce residuals to 1e-7 and the coeficients go slightly better even if it can't converge residuals curve looks quite horizontal (see picture)

I guess I gotta chose the last value of the moment coefficient, when covergence is reached, but Cm oscillates a lot and it can vary 20% of its value (see picture).
Should I use the mean Cm even if it's a steady case?

convergence looks good.

I've tried running the case with a more dense mesh (4 million elements) and convergence is harder to achieve. I had to reduce pressure and momentum URF to their half values and residuals went down. If I try to increase them it diverges.

I'm using a rotating reference frame along axis (0,0,-1) and recording moment coefficient along axis (0,0,1), the issue is that for previous mesh Cm converged to a positive value and now it does for a negative value! I guess Cm should has the same sign as the reference frame rotation, so for that axis negative coefficient should be the right one (see picture for axis and relative flow directions). So how could it have converged to an opossite value?

I also need to meassure lift force for a blade section, but how can I get pressure coefficients along a section perimeter?

Thanks a lot!

Hi everybody,

After some days of simulations I haven't made much progress.

First I've run the laminar steady case. Increasing the windspeed and rotational speed from 5m/s-10rpm, 10m/s-20rpmand 15m/s-30rpm.
Reverse flow appeared and torque coeficient were too low or even of opposite sign.

Now I'm trying the laminar transient case. The mesh is 4 mill nodes. I'm using single precision, SIMPLE algorithm, least squares cell based for gradients, standard for pressure, 2nd order upwind for momentum and 1st order implicit for time.
I'm using adaptive time step form 1e-7 to 1e-3, and residuals of 1e-5. I tried residuals of 1e-6 but they were never reached, and the curve was completely horizontal so I increased them to 1e-5. I've also tried with 1e-4 and 1e-3.

The issue is that I always get reverse flow on the outlet and that ends to distort the flow.

How can I avoid the reverse flow?
Even lager domain?
Should I start with the final windspeed (15m/s) but reduced rotational speed (30rpm=final rotational speed)?
Which approach should I use? Any reference or example?

Thanks a lot guys!

PS: the Cp distribution along a profile of the blade is already solved!

Thats good that you have solved cp distribution problem. Would you like to tell us how you did this?

Do you have separation on airfoil?

Thanks for the theory! But there is still something I don't understand: when we adjust the Flow Courant Number (under Solution Controls), why can we still adjust the URFs? The way I see the equations, the solver uses either the CFL formulation or the formulation. Why can we adjust both?

I created a thread about that, I put the solution there. I did an iso-surface on my specified wall zone with mesh variable.

http://www.cfd-online.com/Forums/flu...urve-plot.html

I had kind of separation for the steady case. The weird thing is that now, in the transient case the flow seems to go opposite to the correct way!:(

I have a 120º cylindrical sector with periodic sides and I want the flow to go opposite to clockwise sense.

What I'm doing is:
I use rotating reference frame (not rotating mesh) and I set it to rotate clockwise, so the flow relative to it goes the opposite. Is that okay? It seemed to be all right for the steady case but not now!
When I check relative velocity vectors they were okay for the steady case, but not for the transient one. If I check them now, they go just parallel to the rotating axis and absolute velocity goes clockwise!:mad:
What difference is there between rotating mesh and rotating reference frame?:confused:

Anybody with experience doing turbines could tell me how he simulates the rotating flow, please?

Thanks many!

Guess this post got lost in so many email updates from the forum! If you see the methodology of solution here, the CFL is only applied while solving continuity, momentum and energy equations (p, u, v, w, T).

Essentially, when CFL is used, the URFs for p, u, v, w, T shouldn't be available. But the URFs are still used for k and eps etc, as a mathematical closure. While, when CFL is not used, the URFs are available for all the variables.

OJ

Hi oj,

The URFs for pressure, momentum, temperature and energy are definitely still available when the CFL is available as well, nothing is grayed out. And modifying either the CFL or the URFs of p, momentum or T have an effect on their residuals. My conclusion is that both the CFL and the URFs are used by the solver for p, u, v, w or T , but I still don't understand the theory!

Oh well, I think there is a bit confusion over the concept of under-relaxation. There are two types:

1) (Explicit) Under-relaxation of variables: For pressure-based coupled algorithm, this would under-relax the individual variables in inner iterations. Notice that the under-relaxation type for momentum and pressure is EXPLICIT!

2) (Implicit) Under-relaxation of equations: For pressure-based coupled algorithm, CFL applied tries to under-relax the equations through full IMPLICIT coupling. The choice of CFL will influence the local timescale and eventually the solution of the equations, as specified in earlier (long) post. Essentially when CFL is used, the separate under-relaxation of flow equations is not needed. But for turbulence equations, URFs still needs to be specified.

Typical values of Explicit URFs (in pressure-based coupled case) for pressure/momentum being 0.75, it can be further increased to accelerate inner iterations. But for higher order schemes for momentum etc, often it needs to be reduced to say 0.5 etc, with very bad meshes requiring further reduction at times. Any divergence in AMG solver should indicate the high CFL value, which needs to be reduced.

OJ

Fluent recommended CFL number for pressure based- coupled to 200000. And this CFL is only used for the momentum and continuity equations (as they are only coupled in pressure based coupled solver unlike density based coupled solver where continuity, momentum and energy are coupled).

So 200,000 does not make a sense as CFL number :confused: but it is doing the great job :o

Indeed, as I outlined, CFL is used only for flow equations (p/v) since only they are coupled, while turbulence and other equations are segregated, even in coupled solver.


The high recommended value of CFL (200000) can be justified in the sense that given the fully implicit coupled equations, this will use relatively quite high timescales locally, accelerating the convergence as information propagates at faster rate. This should be possible because of the implicit nature of coupling and hence no barrier on timescale. Although, the non-linear outer iterations may put a cap on CFL.

That said, I don't know where this figure of 200000 comes from. I remember to have seen reference where CFL was recommended as 1e7 for transient cases (with explicit URFs 1) in FLUENT documentation. Have you read any study which recommends this (CFL=200000)?

OJ

yes. It was a paper on transition model where energy equation was not solved on low pressure turbine and CFL was taken to be 200,000 We are using coupled pressure solver with CFL = 200,000 successfully for few years and convergence is great.

To take this opportunity I would like to share my recent experience. I solved flow around cylinder at Re = 40. At the Re flow is laminar, steady and exhibits two steady vortices in wake region. When I used SIMPLE method, it took around 400-450 iterations to converge solution to required Cd values while in coupled pressure based solver with CFL=200,000 it only tool 24-25 iteration to get the same result.

I see. Indeed, coupled solver will be faster in terms of number of iterations because, of course it solves implicit coupled equations. But be aware that the memory requirements can be a bottleneck in this case. Moreover, time/iteration is significantly higher for coupled solver in many cases.

In cases, where CFL number has to be significantly reduced to aid in convergence, it may be worthwhile to go for segregated solver instead.

OJ