Thermal specification for CHT.
I have been doing Conjugate Heat transfer problem. Here One solid block is put inside one bigger block. The fluid flows from the bigger block. My understanding is that, by specifying boundary conditions on the surfaces of bigger block (from where fluid is flowing), I can get temeperatures on the solid wall. But, in STAR CCM+, by default the walls need thermal specification. I think that, this should be the output. I mean, I need to get temperatures on solid block walls, then why shoud I specify thermal specifications (Adiabatic, temperature, Heat flux etc etc). Please clarify this, if anyone knows. I have attached the image.
Thermal specification for CHT. Reply to Thread
Why you do not work with the heat source in the small block.
When you calculate CHT between the fluid and the solid, you have no wall (in the sense of a BC) between the solid and the fluid but an interface that does not need any thermal specification.
If you don't want to model the solid block and have walls instead then you have to give the code some more information (i.e. a thermal specification) to get a meaningful answer.
hope that helps,
I have the same problem.. I need to define a coupled boundary condition for the walls, but all I have is heat flux, convection ..
Is there an equivalent wall thermal specification in STAR_CCM+ which basically works as a coupled boundary as in FLUENT, while simulating conjugate heat transfer?
First try to understand what CHT means before setting boundary conditions
Guys, it seems there's some clarification needed.
CHT = conjugate heat transfer. That means, you need to have two different bodies as CHT means, you model the heat transfer from one body to the other one. Let's say, one body is a hot solid (pot on a cooker), the other one a cold fluid (water inside the pot). And you want to model how the water heats up due to heat transfer from the pot.
You have to build your two bodies. Then you have to create an interface at EVERY boundary where you want heat to pass from one body to the other one. In this case, at all faces where the fluid touches the inner side of the pot. IT WILL NOT WORK WITHOUT INTERFACES!
When the simulation starts, the interfaces will be initialized and all faces in the wall boundary which is connected to the interface will be transfered to the interface. That means, the former wall boundary is empty, there are no faces inside, as all faces are moved to the interface which connects the two bodies. The thermal specification you tried to set can no longer work, since the boundary is empty. This is no issue, since the two adjacent cells on fluid and solid side are now connected and the usual energy conservation equation is solved: Heat flux out of the solid cell equals heat flux into the fluid cell.
The thermal specification works only for boundaries which are not an interface. For example there will be a heat flux the bottom side of a pot due to the cooker. You can put the temperature or heat flux specification at this boundary, so you don't have to model the whole cooker. But this has nothing to do with the boundary where the heat goes from the solid to the fluid, because the heat flux from fluid to solid is a result of your simulation, not a boundary condition (otherwise you wouldn't need a CHT case).
You can also model only a single body, let's say the water contained in the pot. When you know the temperature of all walls or the heat flux, you can put this values and don't have to model the solid. But this is NO CHT simulation, because there is no second body connected.
This works for simple cases when you've got all heat fluxes or temperatures at the boundaries - but for a complex case, it's nearly impossible to have all boundary conditions. That's the point when you start to model the solid as well as the fluid and get a CHT simulation.
Thank you for your usefull information.
But How can we see the influence of the Air convection on our body if we cannot specify anything in our boundary conditions?
consider we have a block which has interface to Air.we should specify for thermal condition of the surface of the block to : convection(with an ambient temperature)
This surface has interface to Air..after runing how can the convection can be considered?
Thank you in advance.
The transport of heat from surface to air by convection and conduction is taken care of by the solver. But you need to specify a thermal resistance on the boundary, and radiation properties if you use radiation.
ooo, read my last post more carefully, it's all written there!
There are two options how to deal with your problem.
EITHER do a CHT simulation. You will model the fluid and the solid, connected with interfaces. The energy transfer from fluid to solid (or vice versa) through the interfaces will be calculated by the solver, and you will need NO boundary condition, except maybe an additional thermal resistance. The amount of heat transferred depends on the thermal boundary layer which is calculated with the flow field.
The MAYBE needed additional thermal resistance only needs to be specified when you want to model something like an additional insulation layer around your block without having to mesh and solve for that insulation layer.
OR you just simulate the solid, without fluid and therefore without any interfaces. Then you need to specify boundary conditions, most propably a convection condition. That's less computational effort, but also less accurate.
|All times are GMT -4. The time now is 07:45.|