[zhaitb]

When modeling a rotating coupling within a stationary cylinder - If I define a single reference frame (for fluid domain), then the option of 'frame change' in the solid-fluid interface should be set as 'none' (since fronzen rotor is used for Multi reference frame). Is that correct?

However, after setting so, a message pump out saying 'the frame change NONE is only valid if the domains on either side of the interface have the same angular velocity'. In my case, domains on either side (rotating fluid & stationary solid) apparently don't have the same angular velocity. Can anyoone explain the seemingly conflicts for me?

discussion4.JPG

[ghorrocks]

I am not sure it will allow frame change across a solid-fluid interface. Give it a try and find out. If it does then you will probably want frozen rotor frame change option.

If it does not allow it then you will have to put a thin segment of stationary frame of reference fluid inside the outer solid and put the interface in that.

[zhaitb]

Thank you for your reply, ghorrocks.

In order to simulate the conjugate heat transfer and find out the surface temperature of the outside cylinder. A 1/4 section is considered. I modeled the solid domain (stationary) and fluid domain (rotating at certain speed). I now have difficulty in the settings of the fluid-solid interface.

I am able to choose the frozen rotor frame change, but what will be the pitch change in my case? the interface is overlapped with each other and I have no idea what is the pitch angle on side 1 and side 2?

I have attache an image for your reference:

Capture.jpg
Capture3.jpg

[ghorrocks]

A 90 degree sector in both regions means your pitch ratio is 90/90 = 1. So set the pitch ratio to 1.

[zhaitb]

So do you mean that I should set Pitch Angle 1=90 degrees & Pitch Angle 2=90 degrees?

Another concern is that do I also need to set the fluid-solid interface (on the fluid side) as 'counter-rotating wall'?

Again some images for your reference:

discussion1.JPG
discussion2.JPG

[ghorrocks]

Yes and probably yes (try it and find check it works).

[zhaitb]

Thank you, ghorrocks.

I monitored the volume temperature in the fluid and solid domain as one of the convergence criteria: volumeAve(Temperature)@fluid. Does that make sence to you and do you recommend other monitor points?

In my case, the volume average temperature keep increasing after 300 iterations (temperature increase about 5 degree C per 100 iterations), do you see what might be the problem?

monitor.JPG

[ghorrocks]

I have no idea what you are trying to achieve with this model so cannot say what are appropriate outputs.

The temperature profile you show is typical when there is a heat input and no heat outputs. So the temperature just keeps going up forever. If the temperature reaches steady state then you need somewhere for the heat to go to.

[zhaitb]

Hello ghorrocks,

The model is a conjugate heat transfer model, in which I am interested to find out the surface temperature of the stationary shroud while a coupling rotating within the shroud.

I understand that I need somewhere for the heat to go to in order to reach steady state. Actually I set 'heat transfer coefficient and outside temperature' on the surface of the shroud, in this way, do you think the heat can eventually dissipate through the shroud to the atmosphere? So that a steady state may reach?

[ghorrocks]

So you have a heat output so it will not heat forever. But have you worked out what the equilibrium temperature will be? Often you can do this as a simple analytical calculation - heat input = heat output where the heat output is the convection condition you are using. It may well be that the equilibrium temperature for your configuration is 1000C.

[zhaitb]

Test shows the shroud temperature is around 110 degree C, in the simulation so far the predicted temperature is about 50 degree C. Then do you think I can initialize fluid domain with an estimated temperature? Say, 60 degree C.

[ghorrocks]

The simulation is showing 50C but rapidly increasing. It is miles away from steady state and it might end up around 110C.

If you only care about the final steady state valve then use initial conditions near that state to get there faster. And you should also use a steady state model in this case as well. That will get there even faster.

[zhaitb]

Originally Posted by ghorrocks

So you have a heat output so it will not heat forever. But have you worked out what the equilibrium temperature will be? Often you can do this as a simple analytical calculation - heat input = heat output where the heat output is the convection condition you are using. It may well be that the equilibrium temperature for your configuration is 1000C.

Hello ghorrocks,

I still have questions in setting thermal boundary condition on the coupling guard. How should I estimate the heat input in this case? There is a coupling rotating within the stationary guard.

Also, do you think I can simply pick a value for h.t.c? Is there a way to estimate it or I need to write an expression for it?

[ghorrocks]

I have no idea what you are modelling so I cannot say where the heat comes from. But you should know this - you should know the heat source, where it travels to and the path it takes to get there. Only when you know what you are modelling can you set up a CFD model to simulate it.

HTC: This is basic heat transfer background knowledge. Do a google search for guidelines on HTC.

[zhaitb]

Thank you for your reply, ghorrocks.

The heat mainly come from air shearing, friction occurs between adjacent layers of air. The air adjacent to the rotating coupling surface has the largest velocity and air adjacent to the stationary wall has 0 velocity.

I now have difficulties in estimating this type of heat generation, can you give some suggestions to me?

[ghorrocks]

CFX has a viscous work model, you can model this heat generation directly. Alternately a simpler approach would be to put a heat source on the air domain to generate the heat if you know the amount of heat generated. Up to you.

[zhaitb]

Hi ghorrocks,

CFX has 4 types of heat transfer boundary conditions:1)adiabatic; 2)Fixed temperature; 3) Heat flux; 4) H.T.C & outside temperature.

In my conjugate heat transfer model, heat generated in fluid domain will transfer to solid domain then atmosphere.

I want to simulate the surface temperature of the solid domain (stationary guard), when choosing boundary condition for this surface (wall), it seems that I can only choose from 3) & 4). However, I won't be able to know the heat flux nor H.T.C before simulation. I only know the outside temperature. Then how can I set appropriate boundary condition for this surface?

[ghorrocks]

If you don't know the conditions on the boundary then it cannot be a boundary condition, can it? You will have to extend your domain further out to include the surrounding air until there is somewhere you know the conditions to impose a boundary condition.

CFX has more boundary conditions then that. There are also radiative boundary conditions (which are only active if you use a radiation model). Also most of the models you list can be given an expression for input. So if you use a heat flux boundary condition you can write some CEL to make the heat flux a function of anything you like, and then you can apply any sort of boundary condition you like (almost).

[zhaitb]

Hello ghorrocks,

I derived an expression for h.t.c which is a function of temperature diffrence:

h=1.2289(Tsurface-Tambient)^(1/3)

Now I try to input this expression as (to make the final units to be W/m2 K)

1.2289 [W m^-2 K^-4/3]*(ave(T)@shroud-300[K])^(1/3) However error messsage 'bad expression value'

It seems that I can only input decimal in [units]? Do you know how I can input fraction in [units]?

1.2289 [W m^-2 K^-1.333]*(ave(T)@shroud-300[K])^(0.333) This expression works

[ghorrocks]

First of all, h does not have the units W m^-2 K^-4/3. So it is correct in giving an error for it. Note that when units are not correct then you almost always have made a mistake somewhere. So there is probably a mistake in your equation.

But if it is an empirical equation without consistent units and you just want to make it work - then do the calculations unitless and add the units later:

1.2289 [W m^-2 K^-1]*((ave(T)@shroud-300[K]/1[K])^(1/3)

Finally: "ave" is probably the wrong average. You probably want an areaAve. You have defined an arithmetic average.