CFD Online URL
[Sponsors]
Home > Forums > CFX

CFX - Solidworks Flow, Impeller comparison

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2012, 16:37
Default CFX - Solidworks Flow, Impeller comparison
  #1
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 5
aerospace_guy_ is on a distinguished road
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 15-25% 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: no-slip 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: k-e 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
Attached Images
File Type: jpg impeller fluid domain.jpg (29.0 KB, 51 views)
aerospace_guy_ is offline   Reply With Quote

Old   March 14, 2012, 18:15
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,879
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It looks like a pretty basic impeller, I would expect separations and similar sorts of non-ideal 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.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   March 14, 2012, 19:05
Default
  #3
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 5
aerospace_guy_ is on a distinguished road
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)
Attached Images
File Type: jpg CFX-blade pressure plot.jpg (72.1 KB, 48 views)
File Type: jpg CFX-vector plot.jpg (76.5 KB, 46 views)
aerospace_guy_ is offline   Reply With Quote

Old   March 14, 2012, 19:09
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,879
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   March 15, 2012, 05:05
Default
  #5
Member
 
Raja_Bhai
Join Date: Feb 2012
Location: UK
Posts: 40
Rep Power: 4
tauqirnawaz is on a distinguished road
Quote:
Originally Posted by aerospace_guy_ View Post


CFX turbulence model:SST, automatic wall function, 10% at inlet

SW turbulence model: k-e model
Is there any specific reason for using two different turbulence models when you are to compare results from two different software?
Secondly did you consider using an extended suction and velocity inlet instead of mass flow in CFX calculations.
tauqirnawaz is offline   Reply With Quote

Old   March 15, 2012, 12:11
Default
  #6
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 5
aerospace_guy_ is on a distinguished road
@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 trouble-shoot 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 turbo-machinery. 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 K-e 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.
aerospace_guy_ is offline   Reply With Quote

Old   March 15, 2012, 18:57
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,879
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
Basically, what you're saying is that I should focus on reducing my actual CFD errors in CFX
That is exactly right You should compare the simulations when both solvers are doing the best they can do - or at least good enough for the level of accuracy you require.
ghorrocks is offline   Reply With Quote

Old   March 20, 2012, 19:51
Default
  #8
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 5
aerospace_guy_ is on a distinguished road
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 free-slip 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, 1e-5 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,
Attached Images
File Type: jpg sphere Cd mesh 1.jpg (92.4 KB, 25 views)
File Type: jpg sphere Cd mesh 2.jpg (85.6 KB, 21 views)
File Type: jpg sphere Cd mesh 3.jpg (95.2 KB, 17 views)
File Type: jpg sphere Cd mesh 4.jpg (96.4 KB, 16 views)
File Type: jpg Cd vs Re graph.jpg (51.9 KB, 19 views)
aerospace_guy_ is offline   Reply With Quote

Old   March 21, 2012, 00:06
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,879
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
Any ideas what I may have missed
Here's a few ideas I suspect you missed:
* 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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Flow Analysis tilting Pad thrust bearing using CFX julien CFX 5 April 9, 2014 09:38
CFX Coronary Flow Simulation ld1305 CFX 13 February 7, 2012 04:17
How to Check Mass Flow Rate in 2D Analysis - CFX nasir FLUENT 0 October 9, 2011 03:52
How to set pulsatile flow in cfx? bmdaortiz CFX 4 September 8, 2009 23:48
in CFX, how to define a inlet condition of feedback control flow rate ? suihenry CFX 12 May 14, 2009 18:59


All times are GMT -4. The time now is 23:08.