[cfd seeker]

Hello all,

i am doing analysis of a hydrodynamic journal bearing in which the shaft moves at very high rotational speed. The initial temperature of oil and walls is e.g 20 °C (this is all I know about the heat transfer boundary conditions).

When the shaft rotates, then due to internal friction of oil it gets heated and there is a heat transfer to the walls. As I have set the wall temperatures to fixed temperature of 20 °C, it remains the same when i see the results in CFD Post. Now how I can see in CFD Post that how much the walls get heated due to the heat transfer from the oil.

So my question, how i see the temperature distribution (tempetaure rise) on walls because of heat transfer from oil to walls?

Regards

[Opaque]

The following is general heat transfer, not ANSYS CFX related.

You have a system at an initial temperature, and a heat source. Once the journal reaches a steady angular velocity, the heat source will remain constant.

Now you need to assume a boundary condition on the walls to complete the model.

Say you pick a Dirichlet type condition, your fixed temperature:
- you run the model
- Once converged, you can evaluate the heat transfer through the wall
(areaInt(Heat Flux)@Wall in ANSYS CFX speak).
- Such value is the amount of heat that MUST be removed so that fixed temperature can be maintained --> Heating load to your cooling system.

Say you pick a Neumann type condition, i.e. Heat Flux condition
- you run the model
- once converged, you can visualize the temperature profile.
- Such temperature values are the values your journal wall would be at if your cooling system can "really" remove that must Heat Flux.

Say you pick a Robin type condition, i.e. convective heat transfer condition (transfer coefficient and external temperature)
- You run the model
- Once converged, you can evaluate the heat transfer through the wall, and visualize the temperature at the wall
- That will be the temperature of the walls, if that amount of heat flux can "really" be removed by a cooling system at the specified external temperature if the cooling system can maintain/provide such heat transfer coefficient.

Which to model to use depends on what your goal with the simulation is.

[cfd seeker]

Thanks for your detailed reply.

As I mentioned that the whole system starts at 20 °C and then due to the internal friction (viscosity) the oil gets heated and that leads to heat transfer from Oil to Walls. So in this case before the simulation I do-not know how much the oil will get heated and therefore I do-not know either heat transfer coefficient or heat flux before hand.

Any idea how i can model this?

[ghorrocks]

Do a CHT simulation which include the outer casing of the device. Then you don't need to calculate a heat transfer coefficient, that is calculated for you as an implicit part of the solution. But this just moves the problem out a step - you then need to define a thermal boundary condition on the outer surface of the casing. You might know this (for instance bodies in ambient air have well known heat transfer coefficients).

This is the general principle for boundary conditions. You have to apply a boundary condition at a location where you know the conditions. If you don't know the conditions then you can't apply a boundary condition there and you must put it somewhere else, and generally this means increasing the size of the model. Also note the further away from the region of interest the boundary gets, the less it affects the region of interest in general. So you can apply a bad boundary condition and not affect accuracy if it is far enough away from the region of interest.

[cfd seeker]

Ok thanks for your reply but as you said it will move the problem a step further, which i want to avoid at first.

Can the Wall Adjacent temperature be taken as approximation of Wall temperature in case of laminar flow?

[cfd seeker]

If I just define the heat transfer coefficient for air and ambient temperature at the walls, without modelling the solid part, is this make sense or this gonna not work at all?

[ghorrocks]

Ok thanks for your reply but as you said it will move the problem a step further, which i want to avoid at first.

This suggests you misunderstood my comment. You have to put the boundary somewhere, and that means you need to know the conditions at that location. So it is impossible to avoid the need for defining boundary conditions by making the domain larger. But what it does do is to make the effect on the region of interest smaller. Once the domain is big enough having a boundary condition with a degree of error does not affect your results significantly. So increasing the domain size allows you to reduce the error.

If you model the fluid region only then you can use convection boundary conditions on the outside. In this case you need to define a heat transfer coefficient and a wall temperature, which is the temperature of the wall.

Whether a convection boundary condition is suitable for your case depends on what you are modelling. It won't include the time lag effect caused by the thermal inertia of the casing, and it won't include the variation in temperature throughout the device. But only you can assess whether these effects are significant enough to be a problem.

[cfd seeker]

Thanks for your reply.

Originally Posted by ghorrocks

It won't include the time lag effect caused by the thermal inertia of the casing, and it won't include the variation in temperature throughout the device.

Can you please explain a bit what do you mean by this"it won't include the variation in temperature throughout the device" ?

Do you mean in the thickness of the wall or on the wall in circumferential direction if the wall is in cylindrical shape?

[ghorrocks]

Can you please explain a bit what do you mean by this"it won't include the variation in temperature throughout the device" ?

This statement was saying that if the oil has a temperature difference big enough that it makes the outer case of the device also show a significant temperature difference then this effect will not be taken into account.

[Munte07]

Hi CFD seeker
I have exactly a similar question, but instead of CFX, I am using Fluent. I hope you have found the answer. Would you please share it here so that I can find the temperature distribution inside the bearing.
Thank you in advance.