[cos2pi]

Hey

I'm trying to make a calculation of heat loss from a certain geometry. Parts of my geometry is insulated and the rest is steel.

I can't figure out if what I have done is correct, since my results are so non consistent.

On the curved surface (part of a cylinder) i have a flow flowing with a certain temperature (390 deg C) and through convection heating up my geometry.

I have put this in by convection film coefficient of 200 and the temperature.

Further I have drawn the free stream air which cools my geometry by convection and radiation (haven't put in radiation - wont work).

Inlet conditions 20 deg C and 1 m/s, pressure outlet.

I have attached a photo. https://imgur.com/a/AW0nKZP

[vinerm]

Hi

You have mentioned that the results are not consistent. But that doesn't explain much about the problem you are facing except that you are not getting good outcome. Could you please be more elaborate?

[cos2pi]

Firstly my model doesn't converge.

And I don't seem to have the heat transfer that I expected.

I have a lot of heat going into the system, but I'm not sure if it gets "lost" from the curved face or the rest where it would by in real life.

https://imgur.com/a/tjkO6RE

[vinerm]

If I rephrase the scenario, it is like this

1. You have a solid object that has heat coming in from a certain surface or a group of surfaces where you have applied HTC and T
2. There is a fluid zone around it where you are simulating the flow, which is supposed to cool it.

Am I right about the above two statements? If not, no need to read further and provide more clarity. If yes, then please check the following

How are solid and fluid cell zones connected? Is it a conformal mesh or non-conformal one with interface(s)? If it has interface(s), are they of coupled nature?

[cos2pi]

I have meshed it with ansys meshing - indeed the mesh could be better but looks somewhat okay.

For the interfaces I'm not really sure, it has been awhile since making CFD. I have posted some pictures

https://imgur.com/a/EfGbJcQ

https://imgur.com/a/atuVLdl

[vinerm]

That's what I was worried about. You have interfaces that are not coupled. I would suggest going back to DM or SCDM or whichever modeling tool you use to ensure that all bodies belong to same assembly. If it is DM, then select all bodies and form a new part. If it is SpaceClaim, then go to Workbench tab in SpaceClaim and click on Share. This will ensure that at the Meshing stage there is only one assembly containing all bodies. Consequently, you will have conformal mesh and you would not have to worry about the interfaces, which in my view is very bad idea until and unless interface is the only solution, such as in moving mesh.

If you do not want to do that, then delete the interfaces and recreate them. While creating, ensure that coupled is selected and not mapped.

[cos2pi]

Hi

Thank you for using your time on my problem.

I have made the geometry one part, and imported again.

Should I do something to let the faces know that there is convection from them.

[vinerm]

Fluent will create solid-fluid or solid-solid coupled walls where the overlap exists. If there are portions of the boundary where overlap does not exist, those are treated as external walls. At those walls, you may apply a thermal boundary condition. Default, as you may know, would be adiabatic