[Alex song]

hi dear all~!

I am new to star ccm+ and not good at English.

I only want to calculate the thrust and torque of a propeller in open water condition.

so I'm currently attempting to model the flow through and around the propeller in star ccm+.

firstly, I imported KP505 blade and hub .stl files into star ccm+. I then created two cylinder surface around the propeller.

one is a domain cylinder. the other is a interface cylinder. the cylinder size is in the attached screenshot.

next, I performed a boolean subtract operation on the domain cylinder with the interface cylinder and a boolean unite operaion on the propeller with the hub.

and I created 2 regions out of the boolean subtract and the boolean unite.

I created "interface" out of two regions.

next, I set up a mesh model and condition, physics model(excepting a turbulence model.

I selected the K-E turbulence model) and motion in propeller(Moving Reference Frame), refering to the POW section in the link(http://www.doc88.com/p-3059069150326.html)

I then ran the 3 cases different advanced coefficients J(0.1, 0.5, 0.9).

the result((1-(EFD/CFD)*100(%))) compared with experimental data(Kt,Kq) is within -5%, excepting J=0.9.

it is -93% and -49.6% error, Kt and Kq, respectively at first.

so, I have tried a lot of cases about variable properites (domain and interface size, prism layer setting, Y+, blade and blade tip mesh, interface zone mesh size)

but the result is still -43.35% and -16.09%, Kt and Kq, respectively at J=0.9.

I want to reduce the error within 5% about all advance coefficient(Kt, Kq)

I don't know what I have to do...

I've attached some picture.

Thank you very much for any one could give me a little guideline

[fluid23]

It looks like you have some mesh and maybe domain issues.

1. If you want open water, your domain should be closer to 6-10D. Upstream distance should also be 6-10D and downstream closer to 10-15D.

2. I would choose a symmetry condition over a slip wall. Same effect but less troublesome with convergence.

3. Mesh growth is too rapid as it approaches and leaves the blade region. there are settings that you can use to slow this transition.

4. The bottom right picture shows a very very poor transition from your prism layers to your larger core cells. Try using a smaller size in your surface mesh, assuming you are not critical on memory resources already.

5. The picture could be misleading, but it looks like your prism layers are all the same thickness... these should grow to be closer to your core mesh size as it gets further away from the surface.

6. The surface mesh on the farfield boundaries (inlet, outlet, slip wall) is way too coarse. I would cut this in half at least.

7. Why are you using the trimmed mesher? Polyhedral cells have more faces and will be better suited for resolving the rotating wake of your propeller. Trimmed cells (cubes) are better for aligned flows

[Alex song]

thank you for the reply.

I'll try that way and post the result.

[Alex song]

hi~! Matt~!

I've found the solution for my problem.

First, as you suggested, I tried that from 1 to 7, but it didn't solve the problem.

so I focused on the interface zone. I created the volumetric controls, and adjusted the grid near the interface zone. It is not fast for the grid growth rate.

also, I think that It is the key for the problem to specify prism layer size on the interface.

so now, the error(Kt,Kq) is within 5% along the advanced coefficient from 0.1 to 0.9.

finally, I really appreciate you reply.

Best regards,
song.

[bmaldi]

Originally Posted by Alex song

hi~! Matt~!

I've found the solution for my problem.

First, as you suggested, I tried that from 1 to 7, but it didn't solve the problem.

so I focused on the interface zone. I created the volumetric controls, and adjusted the grid near the interface zone. It is not fast for the grid growth rate.

also, I think that It is the key for the problem to specify prism layer size on the interface.

so now, the error(Kt,Kq) is within 5% along the advanced coefficient from 0.1 to 0.9.

finally, I really appreciate you reply.

Best regards,
song.

Dear Song Sung Jin,

Nice to know you,
I am newbie in star ccm+.
i am also try to sinulation open water propeller, for my special case is ducted propeller,
i have tried the step in the link same as you have done : http://www.doc88.com/p-3059069150326.html
but i still confuse how to calculate the thrust and torque, because i compared with simulation in Ansys(CFX), there was a toolbar calculate and we could calculated easily,
but different than Star Ccm+, i don't know, how to calculate the thrust and torque, also for showing the thrust and torque curves,
hopefully you can help me,
thanks before,
best regards,
Aldias Bahatmaka,ST

[bmaldi]

Originally Posted by Alex song

hi~! Matt~!

I've found the solution for my problem.

First, as you suggested, I tried that from 1 to 7, but it didn't solve the problem.

so I focused on the interface zone. I created the volumetric controls, and adjusted the grid near the interface zone. It is not fast for the grid growth rate.

also, I think that It is the key for the problem to specify prism layer size on the interface.

so now, the error(Kt,Kq) is within 5% along the advanced coefficient from 0.1 to 0.9.

finally, I really appreciate you reply.

Best regards,
song.

Dear Song Sung Jin,

Nice to know you,
I am newbie in star ccm+.
i am also try to sinulation open water propeller, for my special case is ducted propeller,
i have tried the step in the link same as you have done : http://www.doc88.com/p-3059069150326.html
but i still confuse how to calculate the thrust and torque, because i compared with simulation in Ansys(CFX), there was a toolbar calculate and we could calculated easily,
but different than Star Ccm+, i don't know, how to calculate the thrust and torque, also for showing the thrust and torque curves,
hopefully you can help me,
thanks before,
best regards,
Aldias Bahatmaka,ST

[Nazir426]

Can i get KP505 blade and hub .stl files?

[Alex song]

Hi Aldias Bahatmaka!

I'm sorry to reply to your question late.

but I don't know exactly what is your problem.

so, do you solve the problem??

[Alex song]

Hi Nazir~!

now I don't have .stl files. but if you don't know this website(http://www.simman2008.dk/KCS/kcs_geometry.htm),

maybe It can help you.

best regards!

[LeeJunhee]

Hello.
I entered CFD of the freshman.
This difference was not me introduce the propeller thrust and we estimate the torque using the (STAR-CCM+).
But, advance ratio rises, with an error, causing heavy.That's probably the problem of <arrangement of mesh>
Which mesh upstream and in downstream they focused on should I ?
I want to have the know-how of you guys.
Fluid region = 80M
Prop region = 320M
How do I approach?

[LeeJunhee]

Hello.I entered CFD of the freshman.This difference was not me introduce the propeller thrust and we estimate the torque using the (STAR-CCM+).But, advance ratio rises, with an error, causing heavy.That's probably the problem of <arrangement of mesh>Which mesh upstream and in downstream they focused on should I ?I want to have the know-how of you guys.Fluid region = 80MProp region = 320MHow do I approach?

[Tellur]

Originally Posted by Alex song

also, I think that It is the key for the problem to specify prism layer size on the interface.

Hello everyone,

Was wondering if someone has some insight on this statement. Is it really crucial to include prism layers in the interface of a rotating region? I have been having issues with convergence in a simulation of a ceiling fan in a closed room (no inlet and outlet mind you) and there are some artifacts along with spikes in wind velocity along the edge of the rotating zone. Wonder if not having prism layers is the issue there (I can try but it's late now and I had to ask for advice ).

Thank you in advance.

Kind regards,
Theodore.

[fluid23]

If you are seeing spikes in velocity at the edges of the rotating region then adding prism layers may help. Really, prisms are meant to help resolve boundary layers (which shouldn't exist at a interface), however, they will help to resolve local velocity and pressure gradients that might be causing the problem. You could also probably just refine your mesh at the interface boundary and accomplish the same thing.

[Tellur]

Hi Matt,

Thanks for your reply.

Yes that was my thinking as well, since the interface is not supposed to be a boundary would I need prism layers. I added layers at the beginning by mistake actually and then removed them to refine other areas instead.

I have been banging my head on the wall with this one for a while even though it's supposed to be such a simple case. The damn ceiling fan doesn't seem to develop a downward flow lol. Unfortunately, all tutorials of moving reference in the world seem to be about the inlet/outlet/rotating region holy triad which I don't have so I can't really compare one-to-one. That makes me think it's something to do with my physics.

I did just see a tutorial for a propeller blade, with detailed mesh settings and from the looks of it they were really aggressive on the propeller (fan) surface. I will try my luch with that.

Btw, any ideas on low y+ vs all y+ for k-w sst? My limited knowledge says it shouldn't really matter with sst, as long as y+ is close/below 1?

Kind regards,
Theodore.

[fluid23]

If I understand your question correctly, you are asking if it matters if you use low wall or all wall if your y+ values are <= 1? It shouldn't matter. For regions where y+ is small it will use low wall, for regions where y+ is high it will use high wall and then for regions in between the two it will interpolate. If your prism layers keep y+ less than 1 it will be essentially the same as using low wall.