I want to do the analysis of a 4bladed marine propeller in open water conditions. For this I did modelling of 1blade and gave periodic boundary condition. I have velocity inlet and pressure outlet. I used rotating reference frame for the fluid where i gave the rpm with which the propeller is rotating. I went for SIMPLE algorithm and 1st order upwind scheme for discretization. But I am not getting the required results. Should I make the blade stationary? I think by default fluent assumes it to be rotating along with the fluid in case of giving moving reference frame.

Someone please help me in this regard.

Hello,

I have done same computations a month ago and the results I got were good. In fluent, you have two options either - a) you keep the blade stationnary because as you said by default fluent assumes the blade is rotating or -b) you set a rotating motion for the blade.

Actually, I adopted the second choice. then, you can define in the Boundary conditions panel, the blade as "A moving wall", "RELATIVE TO ADJACENT CELL ZONE", "Rotationnal SPEED = ZERO". And also do not forget to adjust the ROTATION-AXIS ORIGIN and DIRECTION.

I started my computations with the first order discretization scheme, and when all the forces became stable I switched to the 2nd order scheme and I continued the computations (without doing any initialisation. There is only a small difference in Kt and Kq values computed with the 1st and 2nd order. But a big a difference in the flow pattern around the blade. Second order scheme gives more accurate results.

Also, do not forget to set for the periodic boundary "ROTATIONAL"

Hope it helps,

Tania

r u sure thsi works.

please explain it agian

regards

Dear Tania, Thankyou very much for your message. I will try out what you said. But I have still some more doubts to clear.

In the second case you mentioned, i.e., you set a rotating motion for the blade, I think in that case you may be keeping the fluid stationary. But in that case, I couldn't understand what you meant by "A moving wall", "RELATIVE TO ADJACENT CELL ZONE", "Rotationnal SPEED = ZERO".

Won't the whole thing become stationary in that case? Or is it that the fluid is given rotating reference frame in which we can specify the rotational speed of the propeller and by the above commands, we make propeller rotate along with the fluid at the same speed.

Also, regarding the switching to 2nd order discretization, did you just make changes in the control panel once the residuals became steady and let the iterations to continue?

Please clear my doubts.

Is the fluid rotation in the opposite direction to the propeller rotation?

Dear Sam, yes I am sure it works, I have compared my results with experimental ones and they are good.

Dear Ammu, you can keep the blade stationnary it will give you the same results because fluent wil consider the blade is rotating but IN THE ABSOLUTE FRAME. and this what is really happening.

In my case, I put the blade moving with a zero speed but in THE REFERENCE FRAME that's why I put "Relative to Adjacent cell". and still fluent will consider the blade is rotating in the absolute frame.

I know you will get bit a confused. But to simplify things just Keep the blade stationnary.

And In my case, I had the outer wall (Around the propeller) fixed, which means it doesn't move. So, in the boundary conditions panel, I put the outer wall, "moving wall", "Absolute" with the "zero SPEED". This is wHat Fluent recommends (please check the tutoriel for a FAN)

For the fluid, I set : - the motion type "moving reference frame" - Rotationnal speed is the speed of your propeller - Rotational axis and direction, you don't need to reverse anything.

When all the forces are stable for the 1st order scheme, in solve and controls solutions, change to the second order and then click on iterate to continue the computations.

Hope it helps, Please feel free to ask me if you need more informations.

Tania

Dear Tania,

Thankyou very much for your help. I will try out what you adviced me and if I still have any problem, I will really need your help.

Could my mesh create any problem? I checked the mesh in FLUENT but it did not show any errors. What about shadow faces? Anything I have to do about those? Thankyou once again.

Ammu

Hello,

you should have a refined mesh around the blade and close to the leading edge and trailing edge of the blade. Concerning the shadow faces, fluent creates them automatically when there is a periodic boundaries. you will notice that Fluent merges the two periodic boundaries under ONE name. You don't need to do anything about it.

whish you good luck. And do not hesistate to ask me if you need help.

Tania

wat if the continuiy equation residul is below 1e-03 and diffence bewteen intet and outlet mass flux equal to 0.0015. is this solution considerad converged. although the flow field is very fine and aligned.

note: all resuidual are fluctuating with same period for all varaiables. (wat does this mean to solution)

the convergence is achieved when all THE FORCES ARE STABLE.

In my case, I changed the convergence criteria to 1e-5 because with 1e-3 the forces are still changing and have not stabilized yet.

So, you should check also the forces before stopping the computations, not only the residuals.

what type of forces?

torque and thrust.

Dear Tania, I tried out what u earlier told me. But still the values I get are very low. I left the residual check at default. I thought continuity is what u asked to get stabilized. How do I know if the thrust and torque is still stabilized or not?

Also would it be possible for u to check my case file if I send it to u? I know it is too much to request such a thing, but I can't see any other way. I am required to complete this very soon. Kindly let me know if this will be possible. If not please guide me more because I need your help in doing this.

Ammu

[nvtrieu]

Hi friends,

Are you still working with CFD now?
Can any one teach me how to simulate a propeller step by step?
Thank you for any help!

[A CFD free user]

Originally Posted by nvtrieu

Hi friends,

Are you still working with CFD now?
Can any one teach me how to simulate a propeller step by step?
Thank you for any help!

Hi friend,
There are actually several items you need to consider. Firstly, are you interested in 2d or 3d simulation? Does you geometry let you apply symmetry or periodic boundary conditions? If you intend to use a 3d simulation, then what type of models you want to employ to model impeller rotation? There are several approaches can be used to model impeller rotation, steady-state or transient ones, such as single reference frame( SRF), multiple reference frame(MRF), sliding mesh (moving mesh) and snapshot model. Besides, the appropriate selection of a proper turbulence model is of highly important issue to accurately predict the main flow features inside stirred vessels. So, as you see, there are numerous aspects that should be taken into account to model a stirred tank accurately. You can learn advantages and disadvantages of these models in literature.

I hope it helps

[sohrabmajd]

hi 2 all
I'm new user of ansys that want to use ansys cfx for a ducted propeller.
i can't mesh my model as good as that my solver give me best results.
how can i mesh my model with boundary layers that have fine meshes near propeller and duct and meshes grow slowly linearly with distance from the duct?
I work with ansys workbench and fluid flow(CFX).
thanks