CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

OpenFOAM pump tutorial

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

Like Tree16Likes
  • 10 Post By linnemann
  • 6 Post By linnemann

Reply
 
LinkBack Thread Tools Display Modes
Old   March 18, 2016, 10:23
Default OpenFOAM pump tutorial
  #1
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 481
Rep Power: 17
linnemann will become famous soon enough
Hi all

I hereby give you a complete tutorial case for running a MRF simpleFoam case of a 3D pump with parametric created impeller and volute.

https://github.com/nelinnemann/openf...llerWithVolute

please read the readme for having the correct software installed.
Attached Images
File Type: jpg screen.jpg (37.7 KB, 109 views)
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   March 19, 2016, 12:49
Default
  #2
Senior Member
 
Paulo Vatavuk
Join Date: Mar 2009
Location: Campinas, Brasil
Posts: 158
Rep Power: 10
vatavuk is on a distinguished road
Hi Niels,

Thanks for posting this tutorial. Can you say anything about the geometry? Is it from an existing pump?

Best Regards,
Paulo
vatavuk is offline   Reply With Quote

Old   March 20, 2016, 01:52
Default
  #3
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 481
Rep Power: 17
linnemann will become famous soon enough
Hi

Nope this pump is purely fiction.

Although the dimension might fit with certain small runners.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   March 24, 2016, 16:23
Default
  #4
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 223
Rep Power: 10
student666 is on a distinguished road
Hi,

can you explain what's the meaning of setting flowrate at inlet and velocity fixed vValue at outlet (U) & zero gradient at inlet and 0 value at outlet for P, meanwhile youžre even setting rotating speed?
Can you please explain comparing with other typical bc's for MRF problems?

Can you explain in detail how you choose inlet & outlet values for k and omega? (please don't answer:" use turbulence properties on cfd tools...)

What sort of post-processing analysis would you do to analyze your "fiction" case?

Thanks a lot for your answers.

MC

Last edited by student666; March 24, 2016 at 18:59.
student666 is offline   Reply With Quote

Old   March 25, 2016, 03:47
Default
  #5
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 481
Rep Power: 17
linnemann will become famous soon enough
Quote:
can you explain what's the meaning of setting flowrate at inlet and velocity fixed vValue at outlet (U) & zero gradient at inlet and 0 value at outlet for P, meanwhile youžre even setting rotating speed?
Can you please explain comparing with other typical bc's for MRF problems?
Well when you have a pump you normally have a pump curve that consists of hydraulic head vs flowrate. The other curve you have is the hydraulic shaft power required to rotate the pump. So ideally the flowrate is a table of flow points that you sorta know in advance since you might be working with optimizing an existing pump or are using the scaling laws to generate a new pump from an existing design. The hydraulic head you can get by sampling the pressure at the inlet since it is zero gradient. You could also set a pressure of 0 at the inlet, zero gradient at the outlet and then specify a negative flowrate at the outlet (flowrate is normal to the BC) if that makes more sense in your head. Then you can sample the pressure at the outlet instead. To get the hydraulic shaft power you can add a force samling on the rotating parts to get the moment around the z-axis (this case). You can then turn this into Watt using P (kW) = (M (Nm) * O (rad/s))/1000. You can also get the hydraulic power . from those two numbers you can calculate the hydraulic efficiency and that you can compare to another design you make.

Quote:
Can you explain in detail how you choose inlet & outlet values for k and omega? (please don't answer:" use turbulence properties on cfd tools...)
Well I just set the turbulentMixingLengthDissipationRateInlet and the turbulentIntensityKineticEnergyInlet , so I really do not need to estimate them that much, I use them so if I choose a new flowrate the values automatically adjust. The internalField values are just a starting guess and can be any smaller number.

Quote:
What sort of post-processing analysis would you do to analyze your "fiction" case?
First see above about the hydraulic shaft power and efficiency, next see below for a general observation.

This is where most people in my opinion get CFD wrong, all those color plots are well and nice, but to understand a 3D flow pattern from some 2D plots and vectors are not sufficient to detect a pattern (unless you are very special ). I've had colleagues that told me they had designed pumps (CFD) that had the nicest flow patterns and everything looked perfect, but when it came to prototype testing some of the "worser" looking pumps (flow patterns) performed better than the "perfect flow". All the color plots and streamlines etc. are good for showing at the conferences and to meetings where the boss attends.

So my advice here when doing any kind of CFD, measure or probe things in the case that might be measurable IRL. Those probes and samplings are also a much better indicator that the case have converged than any of the residual plots. I call these values "black body" values as you dont really know what kind of changes influence the result, but they are directly comparable with a number or a curve to another similar design.

The next step is of course to add optimization on top of you parametric 3D case and CFD solution. Then you can do all kind of interesting data analysis as you have a direct correlation between the changes you make to the geometry and the "black body" values you get out the other end.

I see CFD as a tool I can use to design or analyse stuff. Rarely do I go into detail about the flow pattern, unless of-course that is what I want. I use CFD as a relative design study, too see "is this design better than the other design". It is my belief that if you see a trend moving toward a better performance in the CFD, 90% of the time you will see a similar trend IRL. This is of-course a coarse estimate and that number will vary from field to field.

You will almost never be able to get 100% identical numbers between CFD and testing, but if you instead see CFD as a prototyping tool too find trends in design you can avoid a huge amount of prototypes even though the numbers might be of by 10-20% you will most likely in the end still have a better product than you started out with. Then it is up to you to find those empirical numbers between CFD and actual products, that my friend is called experience and it does not come cheap.

I mostly work with products that needs to be produced and that often put limitations on how "creative" one can be about the design. Also the solving time can be a significant factor in how "accurate" the mesh can be and how many details one can include in the design. So it almost always a trade-off between accuracy and time-to-market.

This became a much longer post than anticipated, but I hope you and others get my points.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   June 28, 2016, 11:03
Default
  #6
New Member
 
Max Ng
Join Date: Jun 2016
Posts: 7
Rep Power: 3
maxkcngcfd is on a distinguished road
Hi Mr. Nielsen

what an impressive example you came up above. i'm relatively new to OpenFoam and wanted to investigate the flow pattern inside the pump, which your example make great fit in my need. however, there's one problem thou. i only have window version OpenFoam which prevented me from using 3rd party linux programing like you used in your code. before i jump straight into setting up a new linux OS and then Openfoam. I wonder if it will still be possible to make your case run in window Openfoam? appreciate your reply. thanks!
maxkcngcfd 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
OpenFOAM v3.0.1 Training, London, Houston, Berlin, Jan-Mar 2016 cfd.direct OpenFOAM Announcements from Other Sources 0 January 5, 2016 04:18
Wrong results from motorByke tutorial in OpenFoam 2.1.1 jsc OpenFOAM Running, Solving & CFD 3 April 16, 2013 07:26
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 06:55
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 06:25
Modified OpenFOAM Forum Structure and New Mailing-List pete Site News & Announcements 0 June 29, 2009 05:56


All times are GMT -4. The time now is 05:39.