
[Sponsors] 
April 22, 2012, 08:24 
Water turbine model

#1 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi,
I am currently modelling a water current turbine. I have followed the methods outlined in the ANSYS CFX tutorials using frozen rotor/multiple reference frame approach. The turbine has 3 blades of which I'm only modelling 1 and using periodicity about the rotation axis. 2 domains are being used: a stationary one and a rotating one which consists of a blade and hub (the rotating domain rotates anticlockwise when looking back towards the origin. The boundary conditions are:  a velocity inlet  an opening condition was set at the outlet (0 relative pressure (static) zero gradient)  periodic boundary conditions to account for the additional blades  wall functions applied to the blade and hub  frozen rotor interfaces applied between the two domains Using the setup outlined I can achieve a maximum Cp of 0.3 for a turbine with experimental Cp of between 0.45  0.50. To further investigate I changed the noslip wall condition to a freeslip wall condition for the blade and hub, I also turned the turbulent model off (laminar). I expected the Cp to increase to a value close to 0.5 but it also equaled approximately 0.3. I further increased the mesh density on the blade surface but again no change. I have spent quite a bit of time exploring this already (it's getting frustrating). Any suggestions would be greatly received. Many thanks in advance FMOR 

April 22, 2012, 09:30 

#2 
Super Moderator

There are lot of factors to be considered:
1. Boundary conditions. 2. Mesh resolution 3. Reference values. 4. Turbulence model 5. Wall function vs. integration to wall treatment. 6. Interface type I would suggest you take one problem at a time and then ask the question, so that we can narrow down the problem and provide the solution. 

April 22, 2012, 19:22 

#3 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi Far,
Thanks for your reply, I understand what you outline but I have taken these areas individually previously, but to no avail. I was wondering about the rotation direction of the rotating domain. The turbine is to rotate at an anticlockwise angular velocity (about the zaxis looking towards the origin). Is it correct to specify the angular velocity as positive about the zaxis? Although I agree with your comments, is it not true if you run an inviscid problem (freeslip walls and no turbulence model selected) the losses are at a minimum, the only forces to be resolved are pressure forces acting on the turbine blade face and, the wall shear stress (resolving the boundary layer) is not required (as it doesn't exist in this type model). I have generated several meshes of different densities. I created prism meshes to resolve the boundary layer (integrate to the wall approach) but no change in Cp to a value closer to 0.5. What do you suggest? Is there any obvious problematic areas you can see? Thanks in advance, FMOR 

April 22, 2012, 19:43 

#4 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi Far,
Thanks for your reply, I understand what you outline but I have taken these areas individually previously, but to no avail. I was wondering about the rotation direction of the rotating domain. The turbine is to rotate at an anticlockwise angular velocity (about the zaxis looking towards the origin). Is it correct to specify the angular velocity as positive about the zaxis? Although I agree with your comments, is it not true if you run an inviscid problem (freeslip walls and no turbulence model selected) the losses are at a minimum, the only forces to be resolved are pressure forces acting on the turbine blade face and, the wall shear stress (resolving the boundary layer) is not required (as it doesn't exist in this type model). I have generated several meshes of different densities. I created prism meshes to resolve the boundary layer (integrate to the wall approach) but no change in Cp to a value closer to 0.5. What do you suggest? Is there any obvious problematic areas you can see? Thanks in advance, FMOR 

April 23, 2012, 00:59 

#5  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143 
Quote:
CFX is a viscous solver so must have viscosity. So a simple solution to get started is using a simple turbulence model or a coarse mesh. 

April 23, 2012, 09:46 

#6 
New Member
Join Date: Oct 2010
Posts: 15
Rep Power: 15 
What Turbulence model are you using?


April 23, 2012, 09:50 

#7 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi ghorrocks,
Thanks for your reply. I have set up this model initially with a very coarse mesh and increasing the density until grid convergence was achieved. However, grid convergence was achieved at a Cp value of 0.3! If I use wall functions or if I integrate to the wall the value doesn't change by more than 5%. All forces resolve (X,Y, and Z). I followed all the methods outlined in the ANSYS CFX tutorials... Am I missing something obvious?? Thanks, FMOR 

April 24, 2012, 01:45 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143 
The CFX tutorials show how to acitvate various models. They do not show you how to perform a good CFD analysis.
Have you read the FAQ on this: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F 

April 25, 2012, 14:06 

#9 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi ghorrocks,
Thanks again for your reply. I have read through this previously on countless occasions but is always a worthwhile read! A question regarding rotation direction; my turbine blade is rotating anticlockwise (according to the right hand rule in the positive zdirection), to model this in a rotating reference frame (frozen rotor) I give the rotating fluid domain a positive angular velocity. If I give the rotating fluid domain a negative angular velocity does it represent the blade rotating in the opposite/wrong direction??? Many thanks, FMOR 

April 25, 2012, 14:27 

#10  
New Member
Join Date: Jun 2010
Posts: 21
Rep Power: 16 
Quote:
For cP mismatch;  Have you checked the angular velocity, is it same with experiment?  Have you tried shear stress transport model with boundary layer mesh? 

April 26, 2012, 07:31 

#11 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi altano,
Thanks for the quick reply. I scaled up the turbine size but kept the tip speed ratio constant (as size goes up a velocity must change). Do you think keeping the blade size the same as the blade size in the experiment will make a difference? I understand what you mean, the turbine in the experiment will have a higher angular velocity (rpm) than the scaledup version... I am using a tetra mesh with prism elements to capture the boundary layer. Typically, one of the meshes used for a 20m diameter rotor has a y+ value of <1 with 40 layers, growth of 1.2. The turbulence model used is SST I can replicate the exact experimental conditions, however, I feel the result would be the same.. Thanks, FMOR 

April 26, 2012, 07:40 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143 
It is a bad idea to scale the geometry. There are all sorts of nondimensional numbers at play in your model  Reynolds, Froude, Nusselt and many more depending on what models you are using. You can keep one or two of them constant, but the rest change. The result  your model no longer represents the real geometry.
CFX can easily handle any size geometry. It is not like an experiment where a full sized fan disk would cost a fortune. So model the geometry at the same size, flow and conditions as the experiment. 

April 26, 2012, 07:55 

#13  
New Member
Join Date: Jun 2010
Posts: 21
Rep Power: 16 
Quote:
Last thing, the elbows, flow and pressure measurement devices can disturb the flow in experiment, replicate of these component might be useful for more accurate simulation. In that situation, you may have to model full rotor in transient simulation, to capture transient effect which can change the cP value. Last edited by altano; April 26, 2012 at 07:58. Reason: spell correction 

April 26, 2012, 09:11 

#14 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi altano and ghorrocks,
Again, thank you both. I will work on this immediately and report back soon with results of keeping the geometry in CFX the same as experiment. I will deal with the steady state model for now.... Many thanks, FMOR 

May 4, 2012, 05:30 

#15 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi All,
Update. I have set up a model under the same conditions as the well known experiment (published work), however, I am still half way off the experimental result? I have refined the mesh from a mesh containing 200,000 elements to a mesh containing over 2,000,000 elements with 50 prismatic layers, growth between 1.151.2 and a y+<<1. The results don't change (the design case is the same, best practice guides state that for design cases the wall function will give a good estimation). The turbulence model used is SST. Inlet  velocity (same as experiment) Outlet  opening (0 relative pressure with static pressure option) Farfield  opening/wall (doesn't affect the results) Blade/hub  noslip boundary condition Periodicity  to account for the remaining blades Interface between domains  interface with frozen rotor selected I am quite confident my boundary conditions are good but something is not adding up. Any advice is much appreciated. Thanks in advance. FMOR 

May 4, 2012, 06:01 

#16 
New Member
Join Date: Jun 2010
Posts: 21
Rep Power: 16 
Hi FMOR,
What is your equation which you use for calculation Cp in CFX ? 

May 4, 2012, 06:39 

#17 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143 
When you are converging on the wrong answer it tells you that you have missed an important piece of physics in your simulation. Maybe cavitation? Multiphase flow? Experimental error? Small variations in the real geometry from the intended?


May 4, 2012, 06:57 

#18 
New Member
Join Date: Jun 2010
Posts: 21
Rep Power: 16 
Power on shaft [W]:
((torque_z()@blade)+(torque_z()@hub)+(torque_z()@sh roud))*(angular velocity [rpm])*(0.104712) I assume your rotational axis is Z, the name of regions are blade, hub, shroud. Fluid power available [W]: ((massFlowAve(Total Pressure)@inlet)(massFlowAve(Total Pressure)@outlet))*((massFlow()@inlet)/(massFlowAve(Density)@inlet)) 

May 4, 2012, 07:55 

#19 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi Altano,
Thanks for the reply. C_p=P/(1/2 ρAU^3 ) P=Torque (CFX)×angular velocity (rads/s)×Number of blades Thanks, FMOR 

May 4, 2012, 08:04 

#20 
New Member
Join Date: Apr 2012
Posts: 14
Rep Power: 14 
Hi ghorrocks,
Thanks again for your reply. Where are these errors you outlined displayed? FMOR 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
mass flow in is not equal to mass flow out  saii  CFX  12  March 19, 2018 05:21 
water spray, multhipase model???  bugra  FLUENT  2  February 10, 2010 04:59 
Multiphase model, water disperses in air  bugra  Main CFD Forum  1  January 30, 2010 10:57 
twophase model (water & air)  Jan Bohacek  FLUENT  1  January 2, 2010 10:49 
gas turbine combustor model  HELP!  Phil  FLUENT  2  April 9, 2007 05:05 