CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Rotor Stator air gap of an electrical machine (https://www.cfd-online.com/Forums/cfx/176341-rotor-stator-air-gap-electrical-machine.html)

dracula-007 August 16, 2016 12:11

Rotor Stator air gap of an electrical machine
 
Hello everybody,

I´m trying to analyze the heat flow through an electrical machine. I ran in a bit of trouble while setting up the air gap between the rotor and stator. I set the rotor domain to rotating. Between the rotor and stator domain (solid) there ist the air gap (fluid) domain.

I want the air gap to be a closed system, thus there is no axial flow. I tried to not use an inlet or outlet, but at the end the pressure in the air gap was 0 and there was no velocity. So I added an inlet and an outlet with a very small velocity at the inlet, but it still doesn´t seem the right way to me.

Does anybody know a proper way to set this up?

ghorrocks August 16, 2016 19:54

You have to be careful with incompressible fluids and enclosed domains. Any change in domain size will then cause convergence problems as it has no way of accounting for volume changes.

You can fix this by putting a small pressure opening with ambient pressure in it (which allows it to "breathe" a little, or use a compressible fluid which will just change density a little to account for small volume differences.

dracula-007 September 16, 2016 09:11

Hey,

thanks for your answer!I finally got back to work on the problem. Since I´m using air ideal gas, which should be compressible, an enclosed domain should be fine.
Unfortunately I´m not sure about the boundary conditions. The Domain doesn´t have any in- or outlets, but when I start the simulation, I get an error "Fatal bounds error detected, Variable: Absolute Pressure". I tried to set the Pressure with "pressure level information", but it did´t help.

ghorrocks September 18, 2016 07:46

It means the absolute pressure has gone bezerk. Check your reference pressure. Also, make sure your initial condition is close - if this machine rotates but your initial condition is stationary then there will be massive pressure spikes as it starts to rotate.

dracula-007 September 23, 2016 04:43

Thanks again!

I´m not really sure what I did, but it is working now and I finally got results for my stationary model.

Now I´m trying to do a transient simulation, but I´m not very experienced with that. My rotor is rotating with almost 70.000 rev/min, so the simulation only converges with very small time steps. I read something about 1/omega, but I got to cover 4,2 min. So somehow I got to use larger time steps in order to decrease the calculation time. I´m not sure how to do that. Could it be an option to start with small time steps and decrease them after a while?

Also is there a way to use the stationary solution? I can´t use them as initial values, since the whole system needs to have an initial temperature of 50°C.

Best regards,
Niklas

ghorrocks September 23, 2016 06:04

If you need to do a transient simulation then you are forced to use small time steps with a speed of 70000rpm. So if you do the no-thinking approach of simply a transient simulation for 4.2 min simulation time you will be waiting for years for the simulation to finish.

Or you could be a bit smarter and take a separation of variables approach. Your fluid time scales are fast (fast enough to resolve 70k rpm) and you thermal time scales are slow (minutes). On the fluid time scale the thermal field is essential steady state. So you can assume the fluid stuff can be modelled as steady state at a number of constant temperature states. This will give you a heat transfer. Now you can model the heat side of things with no fluid modelling, just the heat transfer from the fluid replaced with heat transfer coefficients (or what ever is suitable).

This means your all-encompassing transient everything simulation which will be so slow that it will never finish has been simplified to a series of steady state fluid simulations to get the heat transfer, and then applying that to a simply transient thermal only simulation.

AlexRonto October 6, 2016 09:44

Hi Glenn,

I am simulating something very similar (almost the same) and I have the same problem with time stepping in transient analysis. I am doing the smart "trick" you propose, but what I cannot do is

Quote:

Originally Posted by ghorrocks (Post 619026)
Now you can model the heat side of things with no fluid modelling, just the heat transfer from the fluid replaced with heat transfer coefficients (or what ever is suitable).

How can I impose the "heat transfer coefficients (or what ever is suitable)" to a transient thermal analysis?

I suppose it shouldn't be done in CFX but rather at ANSYS Transient Themal?

dracula-007 October 6, 2016 11:42

Quote:

Originally Posted by AlexRonto (Post 620530)
Hi Glenn,

I am simulating something very similar (almost the same) and I have the same problem with time stepping in transient analysis. I am doing the smart "trick" you propose, but what I cannot do is



How can I impose the "heat transfer coefficients (or what ever is suitable)" to a transient thermal analysis?

I suppose it shouldn't be done in CFX but rather at ANSYS Transient Themal?

Hey Alex,

I haven't set the simulation up yet, but I thought about using a constant heat flux (from the stationary analysis) as boundary conditions instead, because I´m more interested in the losses of the air gap while the temperature of the air is changing. You could do that by choosing the boundary "wall" in CFX for the surface of the stator, which limits to the air gap.

Best,
Niklas

ghorrocks October 9, 2016 07:07

If you can average the fluid simulation to a single heat transfer coefficient then it is simple to apply. You can use one way coupling to ANSYS thermal if you need to keep the distribution.

AlexRonto October 12, 2016 10:28

Quote:

Originally Posted by dracula-007 (Post 620543)
Hey Alex,

I haven't set the simulation up yet, but I thought about using a constant heat flux (from the stationary analysis) as boundary conditions instead, because I´m more interested in the losses of the air gap while the temperature of the air is changing. You could do that by choosing the boundary "wall" in CFX for the surface of the stator, which limits to the air gap.

Best,
Niklas

Hi Niklas,

apologizes for my late response.
I'm not sure of what you propose

I am simulating an Axial Flux Permanent Magnet electric generator. 3domains: 1"fluid" domain with atmospheric pressure boundaries, 1 "stator" domain which encloses the 1 "coils" domain. I did not include the "rotors" domain because for some reason CFX could not produce the fluid flow in that case. So, I just set the walls of the rotors as "rotating walls" and by using a transient analysis I managed to get the flow field converged and developed. I set the coils domain to be the constant heat source of about 2000W. What I need is the Temperature at the coils to be calculated by CFX.

My problem is that after different combinations of time steps the Temperature at the coils is stabilized at a much higher value than the one I expect.

The stator, coils and fluid surfaces are not boundary conditions to me, they are Interfaces. So if I set a heat flux produced at the coils' walls (which I think is what you proposed) I leave out the "coils" domain so I cannot get the coils' temperature.

I hope I didn't jumble things in your mind..:)

Alex

AlexRonto October 12, 2016 11:13

Quote:

Originally Posted by ghorrocks (Post 620800)
If you can average the fluid simulation to a single heat transfer coefficient then it is simple to apply. You can use one way coupling to ANSYS thermal if you need to keep the distribution.


Thank you for your answer.

As far as I understand, there are 2 choices for the timescale control strategy at transient analyses:

1)
a)Run a (transient or steady state) simulation with a small time step to get the mass and momentum (and energy) flow fully developed and converged.

b)If the flow characteristics do not depend upon heat transfer, which means that the heat transfer progression through time would not change the pressure and velocities of the flow (which could actually be done if the heat flux affected the fluid density), then a transient heat transfer simulation could be run with initial values taken from the flow simulation and no mass, momentum and turbulence equations been solved. In this case the flow filed is the same for every (large) time step that is used at the heat transfer simulation.

2)
a)Run a number N of steady state analysis with fluid flow and heat transfer equations coupled (N different temperatures for the fluid and the solid domains), by using the "solid timescale factor" to separate the small time steps for the fluid and the big ones for the solids. At each steady state simulation a heat transfer coefficient distribution is estimated by CFX at the fluid/solid interface.

b)Space-averaging the coefficient distribution we get N coefficients.

c)Time-averaging the N coefficients we get a single coefficient which is then inserted to ANSYS thermal to perform an only-thermal analysis.

Is that right?

Thanx again,
Alex

ghorrocks October 12, 2016 18:25

Yes, that looks correct.

dracula-007 October 19, 2016 15:01

Quote:

Originally Posted by AlexRonto (Post 621221)
Thank you for your answer.

As far as I understand, there are 2 choices for the timescale control strategy at transient analyses:

1)
a)Run a (transient or steady state) simulation with a small time step to get the mass and momentum (and energy) flow fully developed and converged.

b)If the flow characteristics do not depend upon heat transfer, which means that the heat transfer progression through time would not change the pressure and velocities of the flow (which could actually be done if the heat flux affected the fluid density), then a transient heat transfer simulation could be run with initial values taken from the flow simulation and no mass, momentum and turbulence equations been solved. In this case the flow filed is the same for every (large) time step that is used at the heat transfer simulation.

Hello everybody,

I tried to decrease the model size by simplifying it (I got from 1/3 to 1/18 of the model by using symmetry). But due to the small time steps I still can´t get the solution in an appropriate time even when I use a computer cluster.

Actually the suggested number 1 is exactly what I planned to do, since some CFD Software is able to do that with just a click. But there´s one thing I´m not sure about. When I´m doing a stationary simulation for the whole model the stator heats up a lot (more than 200 °C). But when I´m using the stationary solution as initial conditions, the stator already has these high temperatures. Is there a way to "override" the temperatures of the Stator to the actual initial temperatures (50 °C) or do I have to do an isolated simulation for the air gap in order to get the initial solution?

Still thanks a lot for your suggestions! :)

ghorrocks October 19, 2016 18:09

Usually you do not model the solid body in these steady state simulations as the solid does not have a sensible steady state result. You replace the solid body with a wall boundary condition on the fluid domain at the temperature the solid body would be at.

Jagan13 August 23, 2022 04:44

Could you please let me know about the boundary conditions you used? did you specify rotor wall as rotating wall or rotating volume all together?


All times are GMT -4. The time now is 11:20.