Hello,

Im new with CFD software and I would like to ask some questions:

I want to analyze a four-bladed thruster propeller with different advance ratio . For this I did modelling fourth of thruster geometry thus one blade and gave periodic boundary condition. I used rotating reference frame for the small propeller-fluid domain where I gave the rpm (1000) with which the propeller is rotating.

-The global domain entrance is defined as inlet (velocity component U=0.5 ms^-1) and turbulent intensity 5%.

-The outer wall is defined as opening with static pressure = 0.

-And the exit also is defined as opening with static pressure = 0.

-I defined fluid-fluid interfaces between the stationary default domain and the small rotating propeller domain.

-The frame change option is set on both fluid-fluid interfaces to frozen rotor.

-The outer wall of the rotating propeller domain uses a fluid-solid interface to the third domain the (I called it) tunel domain (part of the thruster).

I put here some images from my simulations (different inlet speed, different boundary conditions):

--> http://ngrad.bei.t-online.de/UNI/

Now to my questions: -Are these "Pre" settings correct for my purpose (searching forces and moments dependent on advance ratio) or what should I change? -Is it correct how I set up the geometry (e.g. larger area arount the thruster needed) ? -How sould I modelling the rotating domain where the blade extends the rotating domain edge? -Are there any tutorial specially for propeller or impeller simulation available for CFX 5.7?

Any help would be great! Thanks

Zoltan

Hi Zoltan,

I just had a quick look at your set-up and you have the right idea, however a few points may be useful. Very nice idea of putting some jpegs up.....! ;-)

1. These problems are hard for 2 main reasons: the openness of the domain and the "low solidity" of propellers so the flow does not just spin up with the boundary conditons. These both result in some less stable boundary conditons and flow fields than the classical spinning duct stuff!

2. Your mesh looks awful coarse you need a lot of mesh in the theta direction on these guys to get the rignt answer.

3. The extent of the boundaries is pretty close I would like to see boundary regions on the order of 3-5 diameters away to ensure a low sensativity to boundary loction....like everything in CFD you can experiment with this and see how it affects the whole solution. Your inlet distance looks ok...that may need to change with various advance coeff's?? I might put the outlet as just a big hemisphere of what ever radius you choose??

4. Make sure you use the alternate rotation model formulation for this guy and infact you may wish to use a stationary zone inlet regions. The reason there is that the flow is pretty much axial in the stationary frame coming in. If you do this all in the rotating frame then it is highly skewed. The "natural frame" for most of it is stationary.

5. These flows are very sensative to separtation. Check sensativity to turbulence model and inlet values for k and epsilon!

Hope this helps let us know what you find!

Regards,

Bak_flow

Thank you for the answer.

I have enlarged the water area and refined the mesh.

Then I have tried different settings, but I never get the expected results ( e.g. I'm missing the rotating flow out of the propeller area, and the resulting forces are also not realistic). Now I really don't know what I should do, therefore I have made another picture where I described the settings I have made this time.

Could you please take a look: http://ngrad.bei.t-online.de/UNI/Picture001.gif (May be the rotation settings are wrong?)

Thanks Zoltan

Hi Zoltan,

again great idea to show what you have done. I cannot say for sure what is wrong but here are a couple of ideas.

1. I see domain looks ok but am worried that the streamlines at the outer radius of the domain are not very straight and " not just flowing past"....what do you expect.

2. Be very careful on your thrust calculations as upstream of the propeller you do not have an "end surface" included in the domain. This means that even for a hydrostatic case you will integrate over the one end and not the other and have a net thrust! What are your measurements compared to?

3. Comparing to experiments the net change in angular momentum leaving the propeller is essentially dependant upon getting the drag right over the "spinning airfoil" this is usually very hard to get! Very good grids are necessary, trubulence transition may be important, etc. This is infact a hard problem for a simple 2D airfoil calculation. So basically it is not the first number I would look at.

4. What do some of your numbers look like? How did they change when you enlarged the domain and refined the grid?

Just a few ideas......Bak_Flow

Hi Bak_Flow,

I haven't got any measurments to compare my calculations yet beause this propeller exists only in CAD. Maybe at first I should modelling a propeller where measurmets are available to compare with. I hoped that I could get data from the simulation without real measurments but unfortunately what im doing now is more like a blind flight (without any experience in flying).

I have took a closer look at the blade and the pressure does not seams to be ralistic to me:

http://ngrad.bei.t-online.de/UNI/2/Thruster2_003.gif

http://ngrad.bei.t-online.de/UNI/2/Thruster2_004.gif

http://ngrad.bei.t-online.de/UNI/2/Thruster2_005.gif

It might be the problem you described: Getting the drag over the blade. But I have allready refined the mesh in the blade region and the pressure still seams similar to the pressure using a coarse mesh.

"4. What do some of your numbers look like? How did they change when you enlarged the domain and refined the grid?" --->After I refined the mesh the force and torque on the blade havn't changed very much (about +-15%).

Some other screen shots:

http://ngrad.bei.t-online.de/UNI/2/Thruster2_001.gif

http://ngrad.bei.t-online.de/UNI/2/Thruster2_002.gif

http://ngrad.bei.t-online.de/UNI/2/Thruster2_006.gif

http://ngrad.bei.t-online.de/UNI/2/Thruster2_007.gif

The solver manager after 400 iterations:

http://ngrad.bei.t-online.de/UNI/2/Solver_001.gif

So the problem seems to be to simulate the correct drag over the blade. I will again refine the grid. What do you think what else I could do?

Regards, Zoltan

Hi Zoltan,

well it does not look like you are doing too badly.

1. Thruster2-001.gif shows me that those outer streamlines are pretty straight and from this I conclude your domain is large enough.

2. The blade surface mesh does not look too bad although I would like to see some preferential grading at the leading edge/trailing edge. Do you have a boundary layer on it? The issue of getting the drag right will not show up (very strongly) with the pressure field but rather the shear stress field! A really coarse mesh and even an Euler code can get the pressure field close!

I will dig through my stuff and see if there is a nice propeller validation case out there. That is the right place to start.

Regards,

Bak_Flow

Hi Bak_Flow,

I have refined the mesh at the leading edge and made some new calculations. There is a boundary layer on the plane: I use "no slip" conidition and a wall roughness of 10µm.

I have tried different advance ratio: A result of a simulation with 0.5 m/s inlet speed and a very slow propeller rotation (1 rpm) still got a resulting x-force of -7N (negative sign -> wrong direction). That could not be correct. There I realized that I left the front side of the propeller hub(center) open. Therefore the static pressure of this surface area lacked in the simulation result. A just running new simulation shows that the force at the stopped propeller blade is with about +0.2 N (water speed still 0.5 m/s, 1 rpm) really cose to my expected result.

I have asked my old fluid mechanics professor and he told me that the large pressure differences at the leading edge could be correct, because I use a flat blade profile. In this case the complete redirection of the streamlines occures at the leading edge. If I would use a (bent) hydofoil I would also get pressure on the side wall of the blade. Thus for testing I made a new blade and got the expected pressure allocation over the blade surface.

I think that the simulation is getting more and more precisely (thanks to your help). But it would be the best if you could find a propeller validation case because there are still a lot of variables in the simulation I don't know how to set correctly. If you find something could you please send it to my Email adress: ngrad@t-online.de ?

Regards,

Zoltan

Hi Zoltan,

good to hear that things are looking better for your case! ;-)

Yes the issue of including the "ends" is what I was getting at. It looks like you re-did the mesh to include that area. Actually you do not necessarily have to do this. You could just take the net force that results over the one end, shaft, prop, etc and outside of the CFD correct it for the far-field pressure acting on the other end (so long as the end is in the far field)?

Either way you are getting the right idea.

Just an ineresting note for all the people new to CFD out there It is amazing how much one can learn on any application by really digging into the details!

...and the other side of this: how many important details can be missed when we first put a simulation together. ALWAYS, Always, always...have some measurements or analytical solution or somethig for your first problems so that you can spot all the little details that make it work. Once you get to that stage then CFD is really useful!

Speaking of which I will see what I find for validations.

Regards,

Bak_Flow

Hi,

I have searched the web for propeller-relating documents. Because it took a long time to find these information I think this links below can save time for the next one who is interested in this topic.

http://web.mit.edu/13.012/www/handou...rs_reading.pdf

http://www.fluent.com/about/news/new.../pdfs/nl29.pdf

http://cavity.ce.utexas.edu/~kinnas/...d99w/img44.gif

http://www.aem.umn.edu/people/facult...udapest_05.pdf

http://www.nap.edu/books/NI000359/html/511.html

http://www.insean.it/research/ric2/seiun.html

http://www.hydrocompinc.com/knowledg...etricProps.pdf

http://illustrations.marin.ntnu.no/h...cs/propulsion/

http://www.ecadfem.com/fileadmin/fil..._Propeller.pdf

http://pitcairn.fb12.tu-berlin.de/ge...5-2bericht.pdf

http://www.sva-potsdam.de/service/fl...ller/main.shtm

http://www.realtrawlers.com/prop.htm

I have also found propeller geometry data: http://www.nmri.go.jp/trans/Staff/ku...EIUN-pressure/

and a pdf-ducument where this propeller is simulated: http://cav2003.me.es.osaka-u.ac.jp/C...-GS-12-004.pdf

@Bak_Flow:

I want to thank you very mutch for your help.

Regards, Zoltan

Nice Job let us know how your prop works out.

Bak_Flow