# Water turbine model

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 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 no-slip wall condition to a free-slip 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   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54 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 z-axis looking towards the origin). Is it correct to specify the angular velocity as positive about the z-axis? Although I agree with your comments, is it not true if you run an inviscid problem (free-slip 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 z-axis looking towards the origin). Is it correct to specify the angular velocity as positive about the z-axis? Although I agree with your comments, is it not true if you run an inviscid problem (free-slip 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:
 if you run an inviscid problem (free-slip walls and no turbulence model selected)
Free slip walls and no turbulence model is NOT an inviscid solution. It is a viscous solution with free slip walls and a possible unphysical instability due to insufficient dissipation due to the lack of a turbulence model. I do not recommend you do this model.

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.cfd-online.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 anti-clockwise (according to the right hand rule in the positive z-direction), 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:
 Originally Posted by FMOR If I give the rotating fluid domain a negative angular velocity does it represent the blade rotating in the opposite/wrong direction??? FMOR
Yes, exactly. Right hand rule is ok for positive values of angular velocity.

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 scaled-up 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 non-dimensional 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. altano likes this.

April 26, 2012, 07:55
#13
New Member

Join Date: Jun 2010
Posts: 21
Rep Power: 16
Quote:
 Originally Posted by FMOR 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 scaled-up 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
I strongly recommend running with same size with experiment. As Glenn mentioned, it is so difficult to obtain same non-dimensional numbers with scaled model. You should keep in mind that basic model-pyrototype correlations not perfectly worked in real world. Flow separations and other similar phenomena does not occur exactly same on scaled model.

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 1.15-1.2 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) Far-field - opening/wall (doesn't affect the results) Blade/hub - no-slip 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 Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post saii CFX 12 March 19, 2018 05:21 bugra FLUENT 2 February 10, 2010 04:59 bugra Main CFD Forum 1 January 30, 2010 10:57 Jan Bohacek FLUENT 1 January 2, 2010 10:49 Phil FLUENT 2 April 9, 2007 05:05

All times are GMT -4. The time now is 14:40.

 Contact Us - CFD Online - Privacy Statement - Top