[linnemann]

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.

[vatavuk]

Hi Niels,

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

Best Regards,
Paulo

[linnemann]

Hi

Nope this pump is purely fiction.

Although the dimension might fit with certain small runners.

[student666]

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 youìre 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

[linnemann]

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 youìre 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.

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.

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.

[maxkcngcfd]

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!

[CFDpal]

Hello,

First, I want to say Thank you for such good explanations and the cfd case.

Did the author or anyone try running the case in the newer OpenFOAM/Salome/3rd party tools ? Please share your experience.

Salome is 8.3.0 and OpenFOAM is 5.0 now. Do you anticipate any problems in the newer releases of software ?

New installs are typically painful for me and I am afraid since I am novice to Linux.

Thank you in advance.

CFDpal

[maxkcngcfd]

Hi,

I didn't have much luck to get Salome to work (at least on some complex shape like pump it always crash for freeze up) if you are students or working for university, i think you can get a free copy of latest Autodesk CFD.
https://www.autodesk.com/education/f...are/cfd-motion

I would also recommend Simflow
https://sim-flow.com/
they are 3rd party CFD company that develop their own GUI for openfoam. their free license never expired but only allow you to generate 100k mesh. that's a good starting point for you if you are relatively new to openfoam. it really help me to understand alot when i first start learning openfoam.

another software that I came across is CFDSUPPORT
https://cfdsupport.com/openfoam-for-windows.html
this company develop their own window base GUI based on openfoam as well, they do offer 30 days trial and special price for university, try to write to them to get more information.

I also came across HELYX-OS
https://engys.com/products/helyx-os
it seems like they offer free GUI for openfoam in Linux for free, if you operating in window they do offer some support, try to write to them.


last thing that I recommend is try to google "GUI for openfoam"

hope these help.

Originally Posted by CFDpal

Hello,

First, I want to say Thank you for such good explanations and the cfd case.

Did the author or anyone try running the case in the newer OpenFOAM/Salome/3rd party tools ? Please share your experience.

Salome is 8.3.0 and OpenFOAM is 5.0 now. Do you anticipate any problems in the newer releases of software ?

New installs are typically painful for me and I am afraid since I am novice to Linux.

Thank you in advance.

CFDpal

[CFDpal]

Originally Posted by maxkcngcfd

Hi,

I didn't have much luck to get Salome to work (at least on some complex shape like pump it always crash for freeze up) if you are students or working for university, i think you can get a free copy of latest Autodesk CFD.
https://www.autodesk.com/education/f...are/cfd-motion

I would also recommend Simflow
https://sim-flow.com/
they are 3rd party CFD company that develop their own GUI for openfoam. their free license never expired but only allow you to generate 100k mesh. that's a good starting point for you if you are relatively new to openfoam. it really help me to understand alot when i first start learning openfoam.

another software that I came across is CFDSUPPORT
https://cfdsupport.com/openfoam-for-windows.html
this company develop their own window base GUI based on openfoam as well, they do offer 30 days trial and special price for university, try to write to them to get more information.

I also came across HELYX-OS
https://engys.com/products/helyx-os
it seems like they offer free GUI for openfoam in Linux for free, if you operating in window they do offer some support, try to write to them.


last thing that I recommend is try to google "GUI for openfoam"

hope these help.

@maxkcngcfd,

Thank you for your suggestion! However, it is not in line with my goal to use commercial s/w or having limitations on mesh count. I have no problem runing pump cases with comercial packages.

Did you have luck with the abovementioned pump case (not the complex case) ?

Could you please tell some specifics? version of freeze/crush in salome ? Maybe a particular state or step? Did you manage to wmake the application and what OF version? Can you run your app with the mesh? Only the mesh is the problem?


Thank you again for your help!

CFDpal

[maxkcngcfd]

Hi,

it was about 2 years ago, i din't recalled what version of Salome, but it just doesn't allow me to import. every time when i import my step/iges files. the whole program will freeze and after waiting for couple hours it just crash. after trying multiple times, i finally gave up. there's no chance for me to even troubleshoot, I think it simply wasn't design to handle slightly complex 3D files.

i tried to run pump case above but couldn't get it to works as well.

Originally Posted by CFDpal

@maxkcngcfd,

Thank you for your suggestion! However, it is not in line with my goal to use commercial s/w or having limitations on mesh count. I have no problem runing pump cases with comercial packages.

Did you have luck with the abovementioned pump case (not the complex case) ?

Could you please tell some specifics? version of freeze/crush in salome ? Maybe a particular state or step? Did you manage to wmake the application and what OF version? Can you run your app with the mesh? Only the mesh is the problem?


Thank you again for your help!

CFDpal

[CFDpal]

Originally Posted by maxkcngcfd

Hi,

it was about 2 years ago, i din't recalled what version of Salome, but it just doesn't allow me to import. every time when i import my step/iges files. the whole program will freeze and after waiting for couple hours it just crash. after trying multiple times, i finally gave up. there's no chance for me to even troubleshoot, I think it simply wasn't design to handle slightly complex 3D files.

i tried to run pump case above but couldn't get it to works as well.

Hi Maxkcngcfd,

Thank you! Now it is clear.

[linnemann]

New link to the cases are

https://github.com/nelinnemann/of-cases

[djason]

Sorry this is a few years on, and I hope you can see it to respond, but could I ask the source of the geometry parameterization routine? I want to extend it to a twisted impeller geometry. And sorry for my layman terminology but sure you know what I mean ..

[linnemann]

Hi

In the Mesh folder there are two script files for Salome.

SalomeImpellerAndInlet.py
SalomeVolute.py

You should be able to see the parameters and how its done in those.

[djason]

Thanks for responding. Yes I have seen the files and successfully built the geometry in Salome. But I want to understand the calculations and I cant read python..
So did you get the maths from a book or so that I can reference, I.e. if you constructed the code it yourself? Or did you obtain the source code from somewhere?

[linnemann]

It was constructed by me based on my experience with Salome and pump geometries.

You can get inspiration in various pump books, but none of them will give you the final answer or code.

Learn Salome/python and read some books about pumps is the only advice I can give you.

[djason]

Ok, I'll do that. Much appreciated.

[unilord]

Hey,

The cfmesh software is not free. Is there any way that you could share a picture of the mesh, so I have an idea of what it looks like?

[CFD_SG_01]

Hello,
Thank you for sharing this work.
I've noticed the use of simpleFoam solver and the MFR properties.
Have you tried to set this case with a DynamicLMesh properties and pimpleFoam algorithm?

Thank you for your reply