[Gert-Jan]

1) 'Velocity in Stn Frame' is the velocity that you would observe if you were standing outside the geometry (then you are in the stationary frame). Meaning that you were able to measure the velocity using LDA or similar.
'Velocity' is the velocity relative to the local frame of reference. For the housing, it is the same as the 'Velocity in Stn Frame' since the housing is standing still. Inside the rotor it is relative to the Rotating Frame. You as an observer would be able to 'feel' that velocity if you were able to be a small particle going with the flow inside the rotating domain.

In this context, you have a domain rotating with 50 m/s, and a velocity of 63 m/s, relative to this 50 m/s. So that makes a maximum possible of 63+50=113 m/s. Therefore your 111 m/s in Stationary Frame can be explained. The liquid is flowing 63 m/s faster than your rotating domain rotates.

So, in CFX it is not impossible, I am not sure if it is physical. You have to find that out for yourself.

2) You do full 3D? Then your approach is ok. Use 'None' where pitch is asked.

3)- Steady state is ok. Try to find a good solution. Then you can always check transient.
- Don't focus on residuals going down. Keep your eye on the imbalances and try to achieve in=out for air, oil & energy.
- Energy can converge very slowly. Therefore it can be convenient to switch off fluids and turbulence massfraction equations for a while (expert parameter: solve fluids = f, solve turbulence = f, solve mass fraction = f) and solve only energy with a large timestep to get an intermediate solution with energy equation that is in balance (in=out). Can speed up things a lot.

- Do you run Total Energy? Start with thermal energy.

[SeVV]

Thank You very much.
I was confused about the interpretation of strn frame and the interface Type because after changing the interface to translation periodicity both the ‚velocity’ and ‚velocity in strn frame’ was almost the same. I’m trying to imagine why?
According to heat transfer, can I set some kind of heat source somewhere on workpiece and see how the outside cooling is able to reduce its temperature? Which value I should go with, Nusselt number, heat transfer coefficent, Ranz Marshall etc.?

[Gert-Jan]

How should I know?

That depends on what is on the outside:
- air with free convection?
- air with force convection?
- a combination?
- cooling water?
- a vacuum with only radiation?
- heat pipes?

Don't expect me to read your mind.......

[SeVV]

Excuse me, ofcourse I’m not. There is air with free convection on the outside. But I’m not sure what I should start with.

[Gert-Jan]

If your geometry was a cube in a room with 20°C, then I would use "Heat transfer coefficient" with

- h at the top 5 W/m2K
- h at the bottom 2 W/m2K
- h at the 4 side walls 7-10 W/m2K.

Your geometry is like a cilinder. I didn't check the orientation, but given my values, you should be able to set some reasonable values yourself.
I don't expect a huge effect by the way. I think free convection contribution is negligible in your case. But you can include it. It is (almost) for free.

[SeVV]

Can I somehow calculate the "heat transfer coefficent" for the (AIR|OIL) Fluid Pair model? Is there any equation or tables with approximated values?
Or maybe in case when I do not know the heat transfer coefficient value for fluid pair I should chose the Ranz Marshall or Hughmark model?

[SeVV]

Excuse me but I was in big mistake. I need to treat my case as a forced convection heat transfer. In my simulation I`ve assumed that I have two heat sources: the inner surface of workpiece (c.a. 150 °C - measured without cooling, while dry grinding) and the outer diameter of the grinding wheel (c.a. 50 °C degrees - measured without cooling, while dry grinding).
The air from external nozzles (c.a. -2 °C degreeses static temp. set on the inlet) is flowing through the air ambience (18°C) on mentioned workpiece (steel solid domain) and grinding wheel (porous domain). Please see attahced figure where I`ve shown this situation.
The problem is that I`m not sure how to set up the boundaries. I`ve tried few options (fixed temp., heat transfer coefficient and heatr flux) but I am not sure which approach should be better. I want to check the cooling ability of the external nozzle with really coarse precision.
Am I right that there are two following options?
1) I can set the workpiece internal surface to fixed temperature T=150°C and external grinding wheel surface to fixed temp. T=50°C and measure the air near those boundaries to see how much heat flowing cold air has absorbed.
2) I can set the heat source on workpiece internal surface and external grinding wheel surface and check how their temperatures have been lowered by flow of cold air?

According to the second option, I`m not sure how to set the boundaries of heat source, while both of them are interfaces (fluid-solid and fluid-porous interfaces). For example: when I am setting the boundary of the internal workpiece surface (steel, T=150°C) should I set the heat flux (or heat transfer coeffcient) of solid surface or heat flux of fluid (air) surface or maybe both of them? When air fluid is cooling the hot solid I should set the value of heat flux from workpiece (hot solid) to cold air, shouldn`t I?

I`ll be very grateful for Your answer.

[SeVV]

Unfortunately Something is still wrong with my solid-fluid interface. There is no heat transfer between the hot inner surface of funnel and the adjacent fluid wall. It looks like it is insulated and the heat has no allowance to cross the interface surcace.
I`ve tried adding the source on the solid side and adding both the htc and heat flux (in the nonoverlap condition) and still nothing. The only possibility to transfer the heat from my solid to the fluid is to add the source on the fluid side of interface but I think that it is not what I want to achieve. I`ve thick the "heat transfer" option in interface settings. The mesh connection is set to GGI. What else could I check to provide the heat transfer from solid to fluid through the solid-fluid interface?

[ghorrocks]

Then something is wrong with your solid-fluid interface. Check the faces overlap accurately. There is no point adjusting the interface conditions and adding source terms, that is not the problem. Also posting your output file would help.

[SeVV]

Thank You for reply. Here I am attaching my last output file, mayby it would be helpful to judge what`s wrong.
So what is the best way to add the heat source for cylindrical surface? I am adding the source of energy in the 'source' overlap in boundary properties. Changing the nonoverlap boundaries settings (htc or heat flux) has no effort to results. Another way is to add the subdomain and set the volume as a source, am I right?

For something completely different, my convergence is achiving about 1e-5 RMS value and I hope that it`s enough. I don`t know why the curves starts to get ragged as in attached picture and I have ono idea why. I was reducing the timestep from 3e-5 even to 1e-5 and reducing the oil mean diameter but I was still more or less ragged.

[ghorrocks]

The "ragged" convergence is discussed here: https://cfd-online.com/Wiki/Ansys_FA...gence_criteria

You should do a sensitivity check to determine if 1e-5 is tight enough. It may also be tighter than you need, you won't know unless you check. Run 1E-4 and see if it makes any difference to parameters you care about. If the parameters are the same within a tolerance you are happy with then 1E-4 is acceptable.

You do not put sources on surfaces to make them an interface. You use interfaces. There is something wrong with your interface.

[SeVV]

Thank You Glen.
I was checking the differences between results of 1e-4 and 1e-5 RMS and it was not significant difference for results I am interested in.

I understand that for getting the interface we need to insert the interface boundary and it is clear to me. But then we are getting two sides of interface boundary (for example solid side interface and fluid side interface). In my case I want to put the heat source on the solid side of interface (internal sleeve wall). The solid domain is being heated but the air inside the hot sleeve isn`t as warm as I`ve expected (it is rather cool). But maybe if everything rotates with huge velocity (2500 rad/s) and external nozzles delivers the -2C temp cool air it is correct that air inside is not being heated much due to hot solid sleeve internal surface..? I am attaching picture of cross section.

[ghorrocks]

Good to see you have done a simple convergence criteria sensitivity study. It shows you can use the 1E-4 convergence criteria, and that will make your simulations a little bit easier. Have you done also done this for your mesh size? The image you show appears to show a blocky temperature profile and this is the sign of a very coarse mesh - and very coarse meshes are likely to be highly inaccurate and give bizarre results.

It does not matter if you put a heat source term on the fluid or solid side of an interface as they are coupled together and have the same temperature anyway.