CFX  Solidworks Flow, Impeller comparison
1 Attachment(s)
Hi All,
I have an interesting problem here, I am comparing results from a basic impeller simulation between SolidWorks Flow and CFX 12. I'm comparing results from both programs to basic hand calculations. I know that there is going to be some error between the hand calculations and the CFD simulation, so I am looking for comparable results in the range of 1525% error. The problem that I am having, is that SolidWorks Flow, which is usually less accurate, is hitting the hand calculation results almost bang on. The impeller efficiency according to SolidWorks is 98% (based on torque obtained from the simulation), while the percent error between SolidWorks and the hand calcs is only 12%. When I run the exact same geometry in CFX, what I get is much different, the pump efficency is 89%, and the results are showing 78% error from the hand calculations. Both simulations: working fluid: water rotating domain: 1440rpm outlet: static pressure at atmospheric pressure impeller walls: noslip walls inlet: mass flow at 250kg/s (absolute frame) CFX mesh: 5mm max edge length 10deg angular resolution; 746000 elements CFX turbulence model:SST, automatic wall function, 10% at inlet SW mesh: 6mm average size mesh, 10deg angular resolution; 851000 elements SW turbulence model: ke model results from SolidWorks: pressure gain: 125.13kPa impeller torque: 212Nm shaft horsepower: 42.9hp water horsepower: 42.2hp results from CFX: pressure gain: 198kPa impeller torque: 370Nm shaft horsepower: 74.8hp water horsepower: 66.58hp I am more likely to trust the CFX results since I know that it takes more variables into account, and is more widely supported and used. I've also used it a lot more before, with accurate results. I'm not sure exactly what might be the problem with my inputs, or solver variable selections. Could my hand calculations be off by more than the +/ 25% claimed in the textbook? They're based on the Euler turbo machinery equations. I've attached a picture of the fluid domain to the post, the inlet is the small circular plane at the top, concentric with the impeller, the outlet is the plane along the outside ring of the domain, coaxial with the impeller. If anyone can think of something that I might be missing, or some parameter in CFX that I haven't used correctly, please let me know. Thanks 
It looks like a pretty basic impeller, I would expect separations and similar sorts of nonideal behaviour with it. I doubt hand calculations can capture this accurately and I have no idea whether SW is any good in this area. But separations should reduce performance, not increase it like your results may suggest.
As for CFX I would look at the flow it predicts and see what there is. Is it believeable? Does it predict separations? Here is a general FAQ on CFD accuracy which may be of interest: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F 
2 Attachment(s)
Thanks ghorrocks,
I'm familiar with that document you posted. I'll take another look over it and see if I've missed anything. I've looked over the results from the CFX runs, they do look believable, in fact the velocity just ahead of the leading edges, when probed in the stationary frame, is almost what I'd expect based on my calculations. There doesn't appear to be any major separation present, there is an area of lower pressure behind each blade, and a very small separated flow just back from the leading edge of the blades on the trailing edge. I've attached a few close ups of the blade. (note this mesh doesn't have an inflation layer on the mesh since the solidworks mesh system doesn't have that and I'm trying to get as close a comparison as possible) 
Matching errors between CFD codes is a path to nowhere. It does not result in "equivalent" simulations for comparison. You should do a proper mesh with inflation layers for the CFX run.

Quote:
Secondly did you consider using an extended suction and velocity inlet instead of mass flow in CFX calculations. 
@ghorrocks
Thanks for being blunt, I think I needed that. Basically, what you're saying is that I should focus on reducing my actual CFD errors in CFX, instead of trying to troubleshoot what feature in CFX might be causing the discrepancy since I'll never find it. Before starting to look for the source of the difference I had been running the simulations with an inflation layer, trying to get the results as accurate as possible, however the results were still on the order of 80% error from the hand calculations. As for the accuracy of my math, I've compared my math to that in two text books, and it seems correct, though both texts admit that the results will be within 25% of a real case. @tauqirnawaz I started out using the SST turbulence model because my understanding is that it was more robust for turbomachinery. When I started to try and compare my results between the two programs, I figured that the mesh differences between the two would cause a greater source of error than the differences between the two turbulence models. I have tried a simulation using the Ke model in CFX, however the results are nearly identical to that using the SST model. By extended suction and velocity inlet, do you mean, moving the inlet further away from the impeller and using a velocity which will produce the same mass flow? If not, I'm not sure what you mean by suction inlet? Thanks for the help guys. 
Quote:

5 Attachment(s)
Thanks again for the help so far,
I decided to start my study again using a more well known and well documented test case before going into further turbo machinery studies. I created a small wind tunnel 0.6m in diameter, by 1.25m long with a sphere at 0.4m from the front of the tunnel on the center axis of the tunnel. The inlet is a velocity inlet, outlet is a static pressure outlet, and the walls are freeslip walls. The sphere has a 6.25mm constant edge length mesh on it, with a 12 element inflation mesh that is 7mm thick. The mesh expands to an element size of 0.05m at the walls. the total number of elements is 180000. I've done a grid dependency study on the size of the mesh, and this is the threshold where the relative error decreased below 5% running the test at Re=10^5 obtaining a Cd of 0.473. I've run a drag coefficient vs. Reynolds number correlation, however what I've observed is that the coefficient of drag seems to vary linearly with the Reynolds number, not like any of the well known data shows. This is nearly the case for SolidWorks as well. Any ideas what I may have missed, I've gotten good convergence, 1e5 RMS, from the simulations, with slightly poorer performance at Re>35000. Do I need to further resolve the boundary layer in the mesh? Am I missing some key piece of knowledge about how fluid solvers work? Thanks, 
Quote:
* At Re<10^5 or so the flow is laminar. Did you use a laminar flow model? * above Re>10^6 so or so the flow is turbulent. * around the 10^5 and 10^6 range the flow has significant laminar and turbulent bits. Did you use a transitional turbulence model? * The mesh refinement required for these different Re numbers is different. The highest Re number requires the finest boundary layer resolution. * Your domain is quite tight on the body. This will cause blockage factor effects. 
All times are GMT 4. The time now is 02:10. 