[bemomb]

Hello, everybody.

I would like to simulate a simplified swashplate pump. It essentially consists of a rotating disc (orange) on which a piston (red) presses axially. In the appendix you can see a sketch. The rotation causes friction at the interface, which leads to heat development. That's why I d like to define a heat source at the interface (w/m^2 or even better w). The problem is that you can only define a volumtric heat source (w/m^3). Does anyone know how to solve this problem?

thanks in advance

[vinerm]

W/ implies a boundary heat flux and that can be applied only at an external boundary. So, you have to make it a wall instead of interface. Since this is a solid-solid interface, the only field transfer is of thermal energy. If that transfer is not required, you can easily make it a wall and apply heat flux. If that is required, then you have to apply it using UDF. That could lead to energy conservation issues if not applied properly though.

[bemomb]

Hey, Vinerm,

Thanks for your answer. The contact area is recognized by Fluent as a wall by default, so it is possible to define a heat flux. But in my understanding a heat flux bc is not the same as a heat source, because with the bc I only define the heat flux that has to pass through, no matter how much is generated.

But I want to define a source exactly on this contact area, in CFX this is possible without problems.

Do you know how to do that (best without udfs)?
Kind regards

[vinerm]

BC and source are different because one is applied at the boundary while the other is taken as volumetric. However, they are one and the same. What you need to provide is the energy in W. Check the surface area of the wall, divide energy by that number, and apply that as heat flux. That's what boundary source in CFX means.

[bemomb]

Thank you very much!!


One last question: Fluent generates two "interfaces", do I need to define the heat flux on both (devided by two) or only on one of the walls?

[vinerm]

At least two participating boundaries or interfaces are required to create one interface. You have to give boundary condition on the all the walls that are created when interface is generated. For the names of the walls, look at interface panel. If there are only two walls, then apply same number on both sides.

[bemomb]

Okay, so if the friction generates a power loss of 100 W, I will define 50 W on the one side and 50 W on the "shadow" side.

[vinerm]

You have to apply 100 W on both. Do note that although Fluent shows two separate names, they are one coupled boundary. Whatever condition you apply at one will automatically be applied at the other.

[bemomb]

Okay, I will do that! Thank you so much for your help!

Grüße aus Deutschland

[vinerm]

If there is no flow, then fluid properties are not required. However, if by no flow you imply no flow boundary, then you have to look at the objective. If the air and oil never mix, as would happen if they are on the either sides of the plate, then you can keep them at constant density without any problem. If the fluid you are considering is the fluid delivered by the pistons, then you may have to consider compressible liquid for the fluid delivered. If it is gas being delivered, then you can use ideal gas.

Keeping it in the Forum, instead of private, will get you more responses. I am a human being and certainly prone to error. In the forum, I can be corrected. Furthermore, the information shared can be used by others as well, provided you wish to share it. If not, I am alright with PM.

[bemomb]

Thanks for your answer and you are absolutely right concerning posting it in forum. I am not sure if you understood what I meant, that's why I made a picture of the case. With no flow I mean no inlet and outlet. The 2 fluids are not in contact and never see each other. The green fluid is the air that is enclosed in the left part of the pump. The yellow part is the rotating shaft.


The red fluid is the oil. The yellow part on the right side is the swashplate (that is also rotating with the same rotational velocity as the shaft).



Heat is generated between the piston(s) and the swashplate as dicussed above.


Now I am not sure how to define the fluids. As I activated gravity I assume that the boussinesq model is active as well. Is it the right way to define the oil as constant density oil or do I need another definition? and how about the air?


Hope you can help


And thanks a lot in advance


Benni

[vinerm]

From your explanation, I can say that I understood it correctly. Boussinesq model is required only if natural convection is important. Since, you have motion of the plate, that might induce more flow within the cavities than the natural convection. Secondly, though the shape of the volume might change for oil yet neither for oil nor for air the total space is being changed, i.e., at any given instant, both fluids are occupying same volume as they do initially. Then constant density is good enough. And with constant density, you do not need gravity.

I suppose the objective of the oil is to lubricate as well as take away the heat. Couldn't understand the objective of air though. It is quite possible that I do not fully grasp the functioning of the device but as far as I know, it is the pistons that compress the fluid. The regions on each side of the plate do not have much function apart from mechanical and cooling aspects.

[bemomb]

Okay, then I guess I didn't understand exactly what you meant in your post from before You're absolutely right with your explanation how the device works. In reality, the swash plate has an angle and through the rotation the pistons are moved axially. They then compress the water and push it out. The head of the pump where this happens is not part of my model because I am only interested in the heat that is created at the piston-plate interface. I designed a plate without angle and thus the pistons don't move at all.

So you're right: either the volume of air nor oil changes, and as I understand that's the reason why constant density is right for both fluids?

And yes, the air has no specific "task" but as the pump is closed, it's filled with air

[bemomb]

Alright now I also understand what you meant with"the fluid delivered by the pistons". It would be water in this case but as I said I don't want to simulate that

[vinerm]

In that case, I suppose the system is fully incompressible, the effect of buoyancy is also negligible. Hence, constant properties for both should work. And gravity has no effect, so, you may neglect that as well.

[bemomb]

Originally Posted by vinerm

You have to apply 100 W on both. Do note that although Fluent shows two separate names, they are one coupled boundary. Whatever condition you apply at one will automatically be applied at the other.

Hi vinerm,

it's me again

I noticed that my heat flux is 200 W when i define 100 W on each side of the wall. I searched for that problem in the ansys help and added a picture of what I found. It says that to couple the walls you need to choose the coupled condition and give the wall a thickness, then define a volumetric heat flux.

Further it says that if they are uncoupled, you can define two fluxes but I guess then they can't interact.

So what would be the right approach for my problem? In reality, the heat is generated between the 2 components and then goes into the two components and, in my understanding, they can also interact (eg if the piston heats up than the plate the heat will go from the piston to the plate)

[vinerm]

If applying 100 W is resulting in 200 W, then, I suppose, you should apply 50 W. In your very first post you mentioned that you did not want to apply volumetric heat flux. I suppose you did not want that because this would require a solid model. But yes, you can assume some thickness and apply volumetric source. Do note that in case you apply some thickness, it becomes important which material is selected for the wall. Secondly, you have to determine the volume based on the area of the wall and the thickness that you apply and then apply the source as 50/volume in cu.m.

[bemomb]

Yes, i also tried it with half of the total flux on both sides but as I said I think this leads to no connection/interaction between the two parts.

It's not that I didn't want to apply volumetric heat generation, I just thought it has to be area-based as it is generated on an area

My idea is to couple the walls so that they can interact, define a small thickness (1µm or sth. like that), and take my oil as material. That way the heat is generated in the oil and can go in both directions. Apart from that, another thermal resistance is added.

Do you think this is a useful approach?

Best regards

Benni

PS: And yes I would divide my W/m^2 by the thickness to get W/m^3

[vinerm]

Yes, that certainly is a good approach.

[bemomb]

Thank you very much!