Model study Check

[Anonymous]

Hello again,

I made a designstudy which aren't very helpful. I designed a little axial turbine with the goal of a pressure difference.
The Inlet boundary is 5 bar, the oultet is a velocity of 3m/s.

After 100 iterations the pressure difference isnt' there. Everywhere is 5 bar besides the impeller. Only in the impeller the pressure decreases.

So I thought, maybe someone can look after my model an the boundary conditions and say why my results aren't good.

Thank you very much !!!

[Jon.Wilde]

Hey,

I can make a few points:

1. Suppress the outer solid from the mesh, saves a little memory
2. Did you check to see the values at iteration 0? All look OK?
3. You would likely need to run this for 1000-2000 iterations with a 3 deg/time step I would think
4. It might help to switch to 'compressible' but keeping the water as 'fixed' - it can just help with stability
5. Leave Intelligent Solution Control off, or CFD might reduce the time step so much, nothing really happened in the 100 iterations you ran
6. Have a think about the Y+ values if you are running with the SST model (they really need to be less than 2)

Hope that helps!

Jon

[Anonymous]

1. I will make this

2. Don't know what you mean ? Made 0 Iteration and which values and where should i check

3. Usally I do at least 800 but here thought the trend is to bend and would not get any better

4. done

5. the Problem is, that sometimes the solver stops when the intelligent control isn't activated and sometimes the other way

6. the Y+ value is at the Start category "Adaption" right? Cause when I want to activate Adaption, the program says that adaption can't be acitvated in transient simulations. But the Max Y+ is 300, but cannot change it

[Anonymous]

to 2. The Pressure is everywhere 5 bar and the velocity at the Outlet is 3m/s.
Shoulnd't the pressure only 5 bar at the inlet and not overall ?

[Jon.Wilde]

1. I will make this

2. Don't know what you mean ? Made 0 Iteration and which values and where should i check

All over, just to be sure CFD is starting where you think - looks OK to me

3. Usally I do at least 800 but here thought the trend is to bend and would not get any better

With 3 degrees a time step (not blade to blade as you have it at 120deg/step) you will definitely need more

4. done

5. the Problem is, that sometimes the solver stops when the intelligent control isn't activated and sometimes the other way

I would think this would stop happening once you have a smaller time step, the model might just be diverging

6. the Y+ value is at the Start category "Adaption" right? Cause when I want to activate Adaption, the program says that adaption can't be acitvated in transient simulations. But the Max Y+ is 300, but cannot change it

Nope, not that. If you go to Solve -> Result Quantities -> Y+, you will then have Y+ available within the results and you could plot it as an ISO surface once the run has completed.

You will also need to set the Wall Layers to be more suitable to SST, something like 10, 0.5,1.2 (as a first estimate). The Y+ really depends on your flow results though. (Ignore the line that says dropping to 1 layer is a good idea 🙂 ).

[Anonymous]

So I made another analyse.
Activated Y+, deactivated the intelligent control, made 3deg/time.

I wanted to make at least 1000 iterations but stopped at 904, because the process wasn't satifactionary to me.
The pressure increases up to 0,4bar. If the pressure would have decrease 0,4bar I would be happy 😄

Y+ is about the hole surface zero. Is it good or bad? It should be under 2 but is zero still ok ?

Can you please have a look at it?
The roation way is right for a turbine. The Profile isn't the best, but the suction- and pressure-side is available.

Thanks!!

[Jon.Wilde]

For the ramp up in the RR I would have something like this (50 iterations)

You can still suppress the outer solids also 🙂

Is your Y+ actually zero?! That sounds strange, it should be small but ideally not zero.

I set this up to run last night as a test, the intermediate results are currently downloading.

[Anonymous]

okay will write down your tips so I can run another one later, when you analysed your results.

Thank you very much for analysing my case 🙂

[Jon.Wilde]

Early days but this looks pretty OK to me, right? 

Manual mesh, RR ramping up over 50 iterations and I suppressed the solid parts. Thoughts? 🙂

[Anonymous]

When the color gradient represents the pressure I'm positive surprised 😄
Is the rotation way correct ?
Are 127 Time Steps representive for the other time steps ? Or is it possible that the pressure changes from side to side?

But why is there such a big difference? Even when I follow all your steps, the pressure seems good at the beginning but then the difference starts sinking and the pressure is higher after the blades.

[Jon.Wilde]

I am using the same rotation as you, I guess all is OK 🙂

Right hand rule, positive z.

The pressure will change a great deal over time.

Pressure usually rises over a pump, maybe that is what is happening here - are you certain that it hits 3000 rpm and is totally flow driven?

[Anonymous]

Okay the rotation is right.

It should work as a turbine so the pressure should sink.
Usually the turbine would be flow driven, but I wanted to see which pressure difference can be achieved with a certain RPM, because the flow driven process needs more time till the end RPM is reached. Maybe the turbine won't hit 3000RPM in real but it would be interessting which pressure can be achieved.

Did you have any results of more iterations than after 127 ?

[Jon.Wilde]

I started over 🙂

I have a question also - should there not be a hub here? Right now, there is a big leakage path right through the centre of the blades, is that OK?

[Anonymous]

okay cool 🙂

Yeah, it's a hubless turbine of a model of a new hubless rim-driven propeller of ships 😉

[Jon.Wilde]

Very cool! 🙂

[Jon.Wilde]

A comment to add here - if the turbine doesn't hit 3000 rpm in reality and we are forcing it to be at this speed with a fixed 3m/s flow rate, might it not be possible that the outlet pressure is higher than the inlet?

[Anonymous]

Nice one 😄
I never thought about that. Maybe you're right! Maybe the turbine isn't able to come near 3000 RPM in this small pipe and with this small velocity.
So it might be better to think about an RPM around 800-1000. This is way more realistic 🙂

[Anonymous]

Another theorie:

When we define a rotation, the fluid must not deliver energy to rotate the blades. When the fluid drives the turbine it could lost a part of its energy. Kinetic flow energy would be "converted" in mechanic energy.

[Anonymous]

Hey Jon,

sorry to annoy you (:D), but did you get any results of your simulation ? Or do you have any aother thoughts on the pressure increase?

In one question of me you said it is possible to change the environment.
When I change the environment (Water)  to for example 5 bar, define an inlet pressure of 5 bar and a velocity of 3m/, is this the right way? Or is the inlet pressure too much ? Because I thought when I change the environment, it is the same like when I stay at 1atm only with 5bar. The difference would be the same.
Any thoughts ? 🙂