# HELP! Experimental & numerical results don't agree

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 20, 2006, 07:13 HELP! Experimental & numerical results don't agree #1 Jenny Rollo Guest   Posts: n/a I am working on a new type of 3D wind turbine and have carried out extensive wind tunnel tests. I have gone through the first stages of modelling, but my results are widely out. For example at wind speeds of 7, my experimental power output is 4.3W, whereas FLUENT gives 45W and at wind speed 12m/s, experimental was 67W, whereas FLUENT gave 1682W which is impossible since the theoretical idea power output is only 635W. I have had technical staff at FLUENT look at my geometry, mesh and procedures and they can't fault it and have no idea what is going on. My y plus values are good, the mesh is sound and I've used a domain of 12 diameters by 5 diameters, which is about right for the diameter of the turbine which is 870mm. The only thing someone has suggested to me, since Power is proportional to the velocity cubed is that the velocity introduced in the b.c's of the model change, so for instance the input is 10m/s, but it increases to 12m/s through the model. The power was measured experimentally using a generator, and the power calcs in Fluent were just the rad/s x total moment about the z-axis. I would love to hear from anyone who may have had a similar problem where although the CFD model appears to be OK, their results have varied widely when compared to the experimental. Thanks in advance for any light someone can throw on this for me.

 April 20, 2006, 09:01 Re: HELP! Experimental & numerical results don't a #2 Bak_Flow Guest   Posts: n/a Hi, Can you explain your domain and boundary conditions in more detail, particularly the side and outlet boundaries. Do you have a stationary inlet zone? It would also be useful to know some details about the solver set-up, mesh, discretization. Thanks, Bak_Flow

 April 20, 2006, 09:48 Re: HELP! Experimental & numerical results don't a #3 Anindya Guest   Posts: n/a Please check the reference values that you are using for the moment and other calculations. By Default, Fluent use a value of 1 for Velocity and Area. You can change that in the Report-> Reference Values GUI. Put the values of Velocity and Area and other stuff as you would like. Maybe it will give better results. Otherwise there might be some other problem.

 April 20, 2006, 10:13 Re: HELP! Experimental & numerical results don't a #4 Chris Bailey Guest   Posts: n/a I used Fluent's kinetic model for air properties in heat transfer and found the properties wrong by as much as a factor of two. When I substituted my own polynomials I got nice agreement with empirical correlations. Fluent tech support said somewhat cryptically that the kinetic model isn't best, I should use "the" (my) polynomial. On this board somebody explained this had to do with my not choosing a large enough number of degrees of freedom (what? can't find this in docs). So, if you map our your air properties over your model, do they look right?

 April 20, 2006, 11:04 Re: HELP! Experimental & numerical results don't a #5 Jenny Rollo Guest   Posts: n/a Thank you for your replies so far. It's 1am here so I will reply more fully in the morning, but just to explain my setup. 1. Cylindrical domain of size 12D x 5D. I have used an unstructured tet mesh of some 900,000 elements 2. Inlet boundary is a velocity inlet, outlet boundary is a pressure outlet and the side of the cylinder is symmetry. The turbine blades and hub are all walls. 3. All surfaces are stationary except for the internal fluid which rotates at the experimental speeds of the turbine. So I've used an SRF model. 4. My viscous model uses k-epsilon realizable model with standard wall functions. 5. I have used a standard pressure solution with both 1st and 2nd order discretization, both of which have converged well. Hope that helps a little... let me know if there are any other parameters I haven't mentioned which would be useful. Thanks again.

 April 23, 2006, 14:12 Re: HELP! Experimental & numerical results don't a #6 Bak_Flow Guest   Posts: n/a Hi Jenny, thanks for the further discription. Although I can't say without seeing this....I really wonder about how appropriate the domain as a cylinder with symmetry bc on the lateral surface. Physically the flow will then be constrained by this outer cylindrical surface...more like a wind turbine in a shroud (with no losses)...rather than streamlines diverging around the blades and structure. If this is a significant effect then the flow is constrained at the boundary and accelerates through the sections where the physical model/experiment would diverge around....this would give higher power output in your simulation than the expriment....so this thought experiment is atleast leading to the same conclustions as you see ;-) Although I have not done wind turbines, most people put big spherical domains on these "flow in open domains" problems...then far-field or pressure inlet pressure outlet boundary conditions on the sphere surfaces. Check out some literature on what others have done. Note there were some comments on here about mesh, yplus or turbulence model...there always seem to be some regardless of the problem...those things are going to affect your results in the 10's of percents.....not whole number factors. If you are out by whole number factors....it is boundary conditions, missing or wrong geometry, blade angles, etc Euler codes, 2D codes, integral models, etc can get you within 30% on most everything (except drag, heat transfer) on flow over a blade...spinning or not! Good luck and let us know what you find........ ;-) Regards, Bak_Flow

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post cuddaloreselvam FLUENT 0 July 10, 2011 08:25 Ahmed OpenFOAM Running, Solving & CFD 9 June 22, 2011 18:59 yfyap Main CFD Forum 4 February 8, 2011 05:44 ado Main CFD Forum 3 October 12, 2000 08:20 Juan Carlos GARCIA SALAS Main CFD Forum 39 November 1, 1999 15:34

All times are GMT -4. The time now is 23:38.