[Shaheer]

Hello below i have attached the first time step view from the fluent time step animation.
As you can see there are small 2 blocks in a fluid body and the problem i am working on is using heated air to heat the wood chunks.
The air is at 800K while the chunks are supposed to be in 300k.
I patched it during initialization witht he 2 chunks having 300 k and well that yielded a bizzar result of it staying in 300 while the fluid flowing over it cooled rather than it warming up.
If i dont patch even from the start its showing that both the wood and the atmosphere is having the same temperature.
The time step is very low in the transient analysis. over all i simulate for 2 s while each time step is 0.01s.
I am expecting something like a gradual heating of the wood chunks, aparently thats not what I am getting.
Is there some error in what i am doing? Or some way to work it out?
Secondly i have to work on the heat transfer coefficient of the system. what is the prime difference between surface HTC and Wall HTC in ansys?

[LuckyTran]

Check to make sure you have a coupled wall at the interfaces of your block and fluid. You might have be specifying adiabatic boundary conditions there.

The surface heat transfer coefficient is the most commonly used definition: the heat flux divided by the difference between local wall temperature and the reference temperature.

The wall function heat transfer coefficient is calculated in terms of the dimensionless inner variables (u*, and T*).

[RodriguezFatz]

Hi, just some ideas: Did you acutally mesh the inner part of the chunks and mark them as "solid"? Normally, if you do the whole workflow with the regular Ansys tools, everything should be set up automatically, such as Lucky Tran mentioned (coupled b.c.).

[Shaheer]

Hi thanks for the reply, yes there was some coupling error and initialitzation issues which i fixed now its working fine atleast so far.
@Lucky thanks for the definition, If i dont specify a reference it then takes the defalt values which are in the respective temperature box as the bulk temperature right? so if i know that at some point of my flow i will have a stabel temperature i can maually put that as the bulk temperature for the HTC right?
Also if its no trouble could you expand on the wall HTC a bit or link me to somewhere if its discussed in details? like when i checked the theory guide i got a bizzare formula of it being a produce of density spccific heat to a certain power and a Cμ to a certain power tirbulent velocity to a certain power and then divided by a dimentionless temperature which i believe you mentioned.
I know μ is dynamic viscosity but whats Cμ? if my flow is laminar how does it calculate the Kp?

[Shaheer]

Hi i followed most of your recommendations and in 2 scenarios where it hosted only one material it worked perfectly, thanks I was trying a more complex model with 2 kind of things, a steel particle and a block of straw.
When i initialize it with the given reference and everything i am getting something like this
**Warning: zone of type interior found between different solids!
Material of cell zone 12 is steel, while material of cell zone 10 is straw.
Warning: zone of type interior found between different solids!
Material of cell zone 17 is steel, while material of cell zone 10 is straw.
Warning: zone of type interior found between different solids!
Material of cell zone 18 is steel, while material of cell zone 10 is straw.
This will adversely affect the solution.
It is recommended that you fix this issue via the TUI command
**

Is this a bad sign ? my design is attached for more clarification the straw and steel balls were not displayed so that it can be better viewed.
Also on the same vein i tried to find the surface heat transfer coef of the straw and well its just gives a blank show there is a color band ie visible htc around the steel balls but nothing around the contour of the straw. Its weird isnt it? since the whole time the straw is the one which gets heated up. To note i tried a transienct animation of the wall heat flux and it shows to be 0 which is most likely why there is no surface HTC.
Is this Ansys messing up? Or what am I doing wrong?

[LuckyTran]

Originally Posted by Shaheer

Hi thanks for the reply, yes there was some coupling error and initialitzation issues which i fixed now its working fine atleast so far.
@Lucky thanks for the definition, If i dont specify a reference it then takes the defalt values which are in the respective temperature box as the bulk temperature right? so if i know that at some point of my flow i will have a stabel temperature i can maually put that as the bulk temperature for the HTC right?
Also if its no trouble could you expand on the wall HTC a bit or link me to somewhere if its discussed in details? like when i checked the theory guide i got a bizzare formula of it being a produce of density spccific heat to a certain power and a Cμ to a certain power tirbulent velocity to a certain power and then divided by a dimentionless temperature which i believe you mentioned.
I know μ is dynamic viscosity but whats Cμ? if my flow is laminar how does it calculate the Kp?

Fluent uses whatever temperature is in the reference pane. You need to set this temperature to the temperature that is consistent with your definition of heat transfer coefficient, absolutely. Recall that your heat transfer coefficient is not defined until you have defined what the reference temperature is. One drawback in Fluent is it's very hard to use a reference temperature that's not a simple constant.

h* is basically the heat transfer coefficient calculated using the temperature of the wall adjacent cell as the reference temperature. Unfortunately, I can't comment on how or whether Fluent actually does this calculation properly for all types of flows and viscous models. The appearance of kp Cμ are coming from the definition of y* (& u*).

[hotboy]

Originally Posted by LuckyTran

Fluent uses whatever temperature is in the reference pane. You need to set this temperature to the temperature that is consistent with your definition of heat transfer coefficient, absolutely. Recall that your heat transfer coefficient is not defined until you have defined what the reference temperature is. One drawback in Fluent is it's very hard to use a reference temperature that's not a simple constant.

h* is basically the heat transfer coefficient calculated using the temperature of the wall adjacent cell as the reference temperature. Unfortunately, I can't comment on how or whether Fluent actually does this calculation properly for all types of flows and viscous models. The appearance of kp Cμ are coming from the definition of y* (& u*).

Dear LuckyTran!

After reading your explanation I have a question that: If I set the different reference temperation we will have the different heat transfer coeffient ?Why the defalt reference temperature in the fluent is 288.16K not 300K or 310K? If I change the value what's the infuence?Thank you very much!

your sincerely hotboy!

[Shaheer]

What if i assign a zone for my reference values. Like say my outlet zone as the reference values. Based on the upstream heat transfer condition the temperature will change. Also based on position in that zone the temperature will change as well. Say higher temperature on the top and lower on the bottom.
Fluent averages this for every time step if i am doing a transient analysis?