topic Re: Need help simulating a centrifugal pump in CFD Forum

Need help simulating a centrifugal pump

grigore.andrei1234 — Mon, 04 Nov 2019 12:00:14 GMT

Hi!

So i am trying for 3 days now to simulate the flow in a centrifugal pump for liquid methane that i designed. I don't have much experience with CFD programs but i feel getting closer to a good result. The pump should recieve liquid methane with a pressure of 3 bars from a reservoir and is designed with a compression rario of 1.8 in mind, so it should raise the fluid pressure to 5.4 bars.

So, i have 2 volumes, one for the pump impeller and one for the rest of the fluid in the casing. I assign rotating region material to the impeller with the correct RPM and liquid methane material to the rest of the fluid. As boundary conditions i use pressure and temperature at the inlet and mass flow rate at the outlet.

I use incompressible and turbulent flow simulation parameters. I also defined a graph for the density variation with temperature for the liquid methane using a second order polynome to interpolate the values.

The inlet pressure boundary condition is 3 bars, but after running the simulation for 100 time steps and checking the results, the pressure in the impeller varies from 50 bars at the inlet to 5000000000(!!!!) bars towards the outlet which is hugely off my calculations!

Any help and suggestions of what i might be doing wrong is greatly appreciated! I can also send my simulation to anyone who wants to get a better look. Thank you!

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Mon, 04 Nov 2019 13:46:35 GMT

Hello Andrei,

i might be able to help you. Can you share your CFZ file in a compressed folder, i will have a look !
THX

Fred

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Mon, 04 Nov 2019 16:53:48 GMT

Hi Frederic,

First of all thank you very much for wanting to help me! I attached the CFZ file containing the simulation setup. The aluminium part is the pump casing and the titanium part is the pump impeller and stationary diffuser.

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Mon, 04 Nov 2019 19:24:56 GMT

Hello Andrei,

Your centrifugal blower look great : )
Regarding to your CFD analysis, there is several thing that does not work.

Will suggest you to run through these two link :

Link #1 (this one is specially important, focus first on part where they speak about the CAD model)
Link #2

It will give you a general understanding of the rotating region and a broader view on how setting these type of analysis.
Try to modify your CAD like it is suggested in the video. You will probably have question at this point, i will be happy to answer it 🙂

Good luck
Fred

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Wed, 06 Nov 2019 22:12:16 GMT

Hi Frederic!

First of all thank you for the links!

I have tried setting up my simulation like recommended in the links sent by you. I extended my intake and outlet volumes to a length 5x bigger than the diameter, i have set the pump impeller to accelerate gradually to the nominal rpm using the table, all non zero boundary condition also increase gradually with the rpm using Picewise Linear method, i refined my mesh and also calculated my timesteps. The problem still persists.

This is the static pressure distribution in my pump after the simulation. As you can see the minimum pressure is almost 60 bars(!!!), even right at the intake where i set a pressure of 3 bars and is just supposed to be a straight pipe. My impeller increases the pressure of 60 bars to almost 1000 bars which would mean it has a compression ratio of 16.6 which is really science fiction stuff.

Also as you can see from this second photo, the flow enters a stationarry diffuser right after exiting the impeller. The diffuser should further increase the pressure of the flow as it is composed of divergent channels trough which the fluid flows, but in the simulation the pressure drops trough the divergent channels. The pressure then proceeds to decrease gradually towards the outlet untill it reaches 60 bars again right at the outlet, but it is supposed to stay almost constant after the diffuser, maybe decrease a little because of losses due to viscosity and pipe geometry, but certainly not by this much.

This third picture is of the pressure distribution in the intake pipe at timestep 10, at which the impeller has 20% of maximum rpm, but still the intake pressure is almost 60 bars which leads me to think all this has to do with me not setting up my boundary conditions properly.

As boundary condition i set an intake pressure of 3 bars because that is the pressure the fluid will have in the reservoir above the pump and an outlet mass flow rate i expect from my pump to deliver from my calculations.

Do you have any idea of what might be the problem or have any other recommendations i can try?

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Thu, 07 Nov 2019 03:40:19 GMT

Hello Andrei,

i will check
can you provide your lastest cfz and a screen shot of your convergence plot ?
Thx
fred

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Thu, 07 Nov 2019 15:23:41 GMT

Hello Fred!

Sure, i have attached to this message the simulation cfz file where you can see my setup. Here is also the last convergence plot which i did not give time to converge properly because i was getting the same odd results as all the times before so i stopped it, but maybe it helps you get an idea as it is.

While running my last simulation i might have discovered what is wrong with my simulation but not how to solve the problem. Let me explain:

Here in these two pictures you can see the pressure gradients from my last 2 simulations. Observe how right after the impeller the pressure stays the same, neither increases nor decreases? I believe my boundary conditions, maybe the outlet one, are not properly set up and the flow simply gets choked right after the impeller, basically like having the outlet pipe blocked, so the pressure just constantly increases as the fluid has nowhere to go.

Maybe you can take a look at my boundary conditions and see what i did wrong there, if that is to be the problem?

Thank you!

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Thu, 07 Nov 2019 20:28:18 GMT

Hello Andrei,

Thank for the detailed answer. Your scenario is now far better than it previously was, good job !

Indeed one of your problem came from your boundary condition :

The first thing that i will recommand is to switch to the steady state mode (for your boundary condition)
1. Right now you have transient BC with a constant value.
The other problem is related to the physic of your system.
1. The 3 bar pressure is due to the hydrostatic pressure when your fluid is at equilibrum. Once you opened the valve, potentiel energy is transfered into kinectic energy. This energy transfert will drive the flow through your system. Static pressure is more like a resistance to your flow. My recommandation for your BC is the following :
  1. Intlet : 0.0238 kg/s (make sure the flow enter the model)
  2. Outlet : 0 bar, if there is no resistance at the exit of your model.
Bernoulli equation might help you to figure it out the magnitude of the flow at the intlet.

Other comment about your cfd analysis :

uncheck the intelligent solution control in the ''control solution'' tab
Usually when i work with rotating region they are surrounded by fluid. in your case there's no fluid around it. I'm not sure if it is a real problem, i just never see a setup like this, so it's more a general observation than a concern for the validity of your cfd prediction.

Hope it Helps
Fred

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Thu, 07 Nov 2019 22:40:54 GMT

Hello Andrei,

i'm pretty sure that your rotating region can not touch to solid material. Fluid must surround your RR

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Fri, 08 Nov 2019 12:34:29 GMT

Hello Fred!

I disabled "Intelligent Solution Control" and also set up the boundary conditions that you recommended. I have also made sure the rotating region volume does not touch the casing and actually stops about halfway between the blade tips and the casing wall. Unfortunately there is no improvement.

Do you think the problem could be from the Materials Property tab?

This is how my materials editor and materials enviorement tabs look like. Should i change something here?

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Fri, 08 Nov 2019 17:43:21 GMT

Hello Andrei,

I run your scenario on my end, and i still have huge pressure like you experienced.

The methane velocity inside the rotating region is really high : around 200m/s in both scenario with 0 and 3 bar pressure at the outlet, respectively.

I check the speed of sound in the methane fluid for the prescribed environment (T=100degK ; 3Bar) i found this :

methane physical propreties

My understanding for a friday afternoon is that temperature will have an impact on the result. So yeah i think you spot the right think here, you should enable heat transfert !

Good Job
Fred

PS : the rotation seems to be setted in the wrong direction according the the orientation of the vanes. Can you confirm, THX

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Fri, 08 Nov 2019 18:20:30 GMT

Hello Fred!

Yes indeed, my impeller should be rotating counter-clockwise, i missed the fact that in the simulation it rotates in the wrong direction, haha 🙂 .

To adress your remark about the high fluid speed in the impeller: yes indeed, the impeller is designed to rotate at 285500 RPM. It has such a high RPM because, perhaps you already observed, it has a diameter of just 16mm. This methane pump is designed for a small liquid fuel rocket. I study Aerospace Engineering and me and some friends want to see if it is possible to make a functional liquid fuel rocket at such a small scale (yes, i know we are masochistic!). So, since the centrifugal pump raises the pressure of the fluid trough centrifugal force, we have to compensate such small impeller diameter with a high RPM so we will have a high enough peripheral speed at the blade to compress the fluid to the value we need :).

I will try to simulate the pump with heat transfer, but before i do that i have a few questions:

1. If i run heat transfer simulation, do i need to unsupress the pump casing and impeller so to allow the program to calculate heat loss trough the walls of the casing?

2. If i do unsupress them, will i need to assign rotating region material property to the solid impeller aswell as the volume around it?

3. Should i also select compressible flow option?

4. Is Autoforced Convection and Radiation necessary? Should i select them?

5. For a heat transfer simulation, are there other result quantities i should select beside these?

By the way, thank you very much for the help so far, i really appreciate it!

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Fri, 08 Nov 2019 19:00:58 GMT

Hello Andrei,

Thank for the specification, seems really interesting project.

In my last post i made a mistake about the heat transfer. You don't need to activate the heat transfer in the physic tab. The software will automatically use the density of the prescribed at the corresponding temperature. (100degK)

Regarding this last point, i think you made an error relatively to the density of liquid methane :

This is the way you setted the physical propreties of the liquid methane

In other hand this is how it is defined on the autodesk database :

autodesk database (liquid CH4)

I check the density dependancy according to the pressure applied at 100degK and there's no significant change :

3 bar = 439.09 kg/m3
2 bar = 439.01 kg/m3
1 bar = 438.94 kg/m3

My interpretation of this is you can use a constant value for the moment and use the methane material in the autodesk database. Right now you have a huge error on the density value.

For the compressibility option, i think you should check the magnitude of your velocity field with the new density values and compute the Mach number to know if compressibility is relevant to your analysis.

Hope it helps
Fred

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Fri, 08 Nov 2019 20:42:17 GMT

Hello Andrei,

Good news !
I finally solve your problem 🙂

Rotating Region is not the appropriate approach in this case. Use angular motion instead !

The physic is really more realistic

They still have ajustement to do but they are minor.

i join my CFZ file
Fred

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Sun, 10 Nov 2019 07:32:34 GMT

Hello Fred!

That is great new indeed! I will try that today and come back with an answer as soon as it is solved 😃

Re: Need help simulating a centrifugal pump

grigore.andrei1234 — Sun, 10 Nov 2019 14:03:12 GMT

Hello Fred!

So i just ran the simulation on the CFZ you sent on your last message and i have to say that it is the biggest progress i have made this far into getting this simulation done!

My impeller seems to compress the fluid to the compression ratio it was designed! But the problem is that it now thinks that the inlet pressure is 80 bars, so instead of compressing it from 3 bars to 5.4, it compresses it from 80 bars to 140-150. Again the compression ratio is more than perfect but the pressure values are off. Also, the flow still looses pressure while flowing trough the divergent channels.

Any idea why this happens? I will also try to experiment with various boundary conditions to see if anything helps.

Thank you!

Re: Need help simulating a centrifugal pump

frederic.gaillard.7 — Sun, 10 Nov 2019 20:00:01 GMT

Hello Andrei,

I'm glad to heard that we make some progress. Your current question is more related to the physic of your model so i will remain cautious about what i'm gonna to say since i don't have the full picture of your project.

From what i understand this a miniaturization of a wider model, what is the scale of this miniaturization ?

Changing dimension will certainly affect the physical propreties of your fluid inside the device.

Since you made a dimensional analysis i will suggest you to read about the Buckingham Pi Theorem to see how physical parameter evolve in a smaller model. However I'm not sure on how to integrate the effect of diffuseur and centrifugal pump.

Fred