CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   STAR-CCM+ (https://www.cfd-online.com/Forums/star-ccm/)
-   -   DFBI problem (https://www.cfd-online.com/Forums/star-ccm/91947-dfbi-problem.html)

 nitin1685 August 27, 2011 06:39

DFBI problem

1 Attachment(s)
Hi,
I am trying to simulate a crossflow turbine in starCCM+ 6.02
see attachement, water is coming from nozzle inlet, and it is flowing from runner blades, I am using DFBI model for free motion of runner, k-e turbulance model. I defined the runner region as DFBI motion and 6 DOF body runner is restricted from all motion except rotation along the z axis.
Still i am unable to get the solution, everytime i have a error of flouting point exception and overflow error.
Physics are- steady state, constant density water, k-e turbulance model, all y+.
head available at inlet is 20 m and mass flow rate as outlet.
What are the possibilities that i can get the rotation?
Also guide me for what possibilities making the runner to restrict the flow?

 sail August 27, 2011 13:32

Quote:
 Originally Posted by nitin1685 (Post 321892) Hi, I am trying to simulate a crossflow turbine in starCCM+ 6.02 see attachement, water is coming from nozzle inlet, and it is flowing from runner blades, I am using DFBI model for free motion of runner, k-e turbulance model. I defined the runner region as DFBI motion and 6 DOF body runner is restricted from all motion except rotation along the z axis. Still i am unable to get the solution, everytime i have a error of flouting point exception and overflow error. Physics are- steady state, constant density water, k-e turbulance model, all y+. head available at inlet is 20 m and mass flow rate as outlet. What are the possibilities that i can get the rotation? Also guide me for what possibilities making the runner to restrict the flow?
mybe is the steady state the problem. as far as i know (but i might be wrong) you need transient simulation to use dfbi.

 abdul099 August 27, 2011 15:12

sail is right, a steady state dfbi simulation doesn't make any sense. When the floating point exception still occurs when running in transient, check the usual suspects: mesh, time step, boundary conditions...

 nitin1685 August 28, 2011 23:31

hi

i did with implicit unsteady state also,
Still i have the same problem.
How to set time step, that i learnt from tutorial.
If any one has good idea about dfbi, please tell tme the unsteady BCs and time step.

 ping August 29, 2011 01:56

DFBI is an overkill motion model for the geometry shown and might not even work - you can use either reference frame motion (and run as steady or unsteady) or rigid body motion (and run as unsteady since the rotor mesh is actually moving).

 nitin1685 August 29, 2011 02:02

thanks,

but reference frame of rotation is only possible when we have rpm of rotor, but in turbines, we want the output as rpm.
In DFBI, we can create the displayer where i think, we can see the actual motion of the runner.
Is it so?

 ping August 29, 2011 02:28

if you want to see the rotor actually move then rigid body motion is the way to do it, and it this case it will be a bit more accurate than MRF, but MRF will get you close an an initial solution in steady mode for the unsteady rigid motion phase.
To solve for rpm you need to do it by trial and error - estimate an initial rpm, run for a while, measure the torque compared to the load on the turbine, if too high, increase rpm etc etc - easy to do in a little macro checking torque every 10-20 iterations or time steps.

 abdul099 September 3, 2011 07:43

ping, DFBI embedded rotation and translation should also be fine. I totally agree with your suggestion, that's what I usually would do. But I disagree, DFBI is an overkill model for this case. That's only true for DFBI morphing!

nitin fixed all motions except Z-rotation. The rotation angle in a time step should be calculated by current rotation rate and additional angle due to angular acceleration from moment imbalance. The mesh will be moved, interfaced and a new time step will be solved.

When running a rigid body motion, the rotation angle will be calculated from the rotation rate and time step. The mesh will be moved, interfaced and a new time step will be solved.

Moving the mesh and interfacing takes the same time as it is the same process. Forces are calculated anyway, and solving one simple equation once per time step for the angular acceleration and the new rotation rate takes less cpu time than surfing in the internet while waiting for results. I'm able to do it by hand, even without a calculator! (of course not that fast like my painful slow Phenom II 965, but I can do it :cool: )

Additionally, it might take a lot of loops of comparing moment and load and adjust the rotation rate, as the load usually changes with rotation rate.

nitrin, does your model run steady state without DFBI? Go from a simple to the complex model. Try to get your model run in steady state (maybe with mrf) without DFBI, then increase the complexity. When it even doesn't run steady state without DFBI, it's not worth to bother about motions.
In my experience, floating point exceptions often come from a crap mesh. And people are spending hours and hours of checking physics although it would make more sense to improve the mesh.
When the mesh is okay, check boundary conditions etc. and get it to run steady state. Then go the second step.

 ping September 5, 2011 07:57

guys believe what you like but a macro comparing torque and changing rmp converges surprisingly fast - used in windwills for example - for anyone who has not tried this technique it is worth a test. has the advantage that you run MRF first then switch to transient and your solution is almost converged already. i'd do both it it was my project.

 abdul099 September 5, 2011 18:22

I always belive what I like :cool:
I haven't said, my solution is the best and only one. I just said, DFBI might also be a solution.

And you should not forget: You made good experience with your approach when simulating windmills. I suspect, there are only minor variations in torque? I tried something similar on a shrouded 3-blade Darrieus rotor with a non-linear power curve, and it took a painfull long amount of time until it reached a quasi steady state.
And for example to simulate the spin-up time isn't that easy with your approach (I know, that's not what nitin asked for, just an example).

It always depends on the case which approach proves to be the best. That's why I'm usually open to all.

 nitin1685 September 7, 2011 07:09

hi

thanks for the response.

I am able to run the CFD.
Unsteady state, DFBI rotation and translation
rotation towards z only.

Its based on time step and run is still going on. So hoping for the best.

Thanks a lot

 abdul099 September 12, 2011 18:47

Sounds great. Time step could be a problem in much cases, but I forget to ask for that very often, as I assume, people would check in on their own as one of the first points... Anyway, good luck for further progress.

 sanchovg2 February 28, 2012 05:08

hello nitin, i know it may be long time ago but did you manage your turbine to rotate and had the rpms as an output? and how was your plot from the body angle? im having troubles with the rotation it goes back and forward...any idea?

 saleh alsubari August 8, 2012 11:42

Quote:
 Originally Posted by nitin1685 (Post 323262) thanks for the response. I am able to run the CFD. Unsteady state, DFBI rotation and translation rotation towards z only. Its based on time step and run is still going on. So hoping for the best. Thanks a lot
can u please send me ur project , i'm really having the same problem ,i need the rpm and the associated torque as in out put..can u tell me what to do,or send me ur project
saleh_nagi2002@yahoo.com

 saleh alsubari August 9, 2012 08:08

Quote:
 Originally Posted by nitin1685 (Post 321892) Hi, I am trying to simulate a crossflow turbine in starCCM+ 6.02 see attachement, water is coming from nozzle inlet, and it is flowing from runner blades, I am using DFBI model for free motion of runner, k-e turbulance model. I defined the runner region as DFBI motion and 6 DOF body runner is restricted from all motion except rotation along the z axis. Still i am unable to get the solution, everytime i have a error of flouting point exception and overflow error. Physics are- steady state, constant density water, k-e turbulance model, all y+. head available at inlet is 20 m and mass flow rate as outlet. What are the possibilities that i can get the rotation? Also guide me for what possibilities making the runner to restrict the flow?
ه

hi ..
did u mange to get it , if yes can u tell me how ? i have the same problem

 Ldugm December 22, 2017 15:09

Can you help, I'm struggling to understand how to have my vertical axis turbine rotating inside the "wind tunnel" - solid primitive block- that I made around it.

I have an estimated rotational speed of 40 rad/s, for a wind speed of 7m/s.

Hopefully you can explain how I set this simulation up, and then how I can find the torqueon the turbine at this wind speed/rotational speed.

 ping December 24, 2017 16:58

first you need to do some cad to create a cylinder around and containing your rotating components - easy in 3d-cad using the boolean tools or in a native cad solid modeller, and a bit harder in parts

now you have two regions and you rotate the cylinder region

torque is measured using a moment report of the blades

 Ldugm December 31, 2017 14:48

Hi sorry for late reply so do I make a second solid primitive, and this time make the dimensions just the max dimensions of the blade? and subtract this from the body as well?

 ping January 1, 2018 14:59

the new solid to be used purely as a cutting tool needs to be larger than the rotation part ie some clearance for at least say 10 cells and preferable bigger on all sides

 Ldugm January 3, 2018 10:54

Hi Ping thanks for all the help. I was wondering if you could help with another problem. I'm trying to run a simulation on the blade as a static problem for simplicity. I have set the inlet velocity to 7m/s, and set up some pressure scenes and moment/force plots.

first problem - my residuals are not going below 0.0001 (some are as high as 1). I have increased the mesh to around 2,000,000 cells and disabled the prism layering at inlet,outlet and surrounding, thinking this would help. however, the residuals are still not converging below the desired value. Is there some other parameter i should maybe be changing that i don't know about? Could it be the size of the wind tunnel? My rotor dimensions are - diameter 0.35m and length 0.7m (vertical axis wind turbine) and so i made the wind tunnel 3mx5mx3m

second problem - For the force plot,i set the direction to be (0.0,1.0,0.0) the y-direction because this is the direction of the flow and i wanted to know how much force the given wind speed is exerting on the blade however it is giving me a negative value for my force.

 All times are GMT -4. The time now is 07:59.