Inconsistency of heat transfer in steady state simulation using Star-CCM+

tjushang · April 25, 2022, 02:53

Hi everyone,

Recently I carried out a numerical simulation using Star-CCM+ which can be described as following:

A cube is put on a cooling plate with rectangular channels. A total heat source of Q1 is set on the cube. The fluid inside rectangular has an inlet mass flow rate of m, inlet temperature of Tin, outlet temperature of Tout. The specific heat of fluid is represented as Cp. Thus the heat taken away by fluid can be calculated by Q2 = Cp * m * (Tout - Tin) in steady state. Other boundaries other than inlet and outlet are all set as adiabatic.

If the described case reaches steady state, then Q1 = Q2 in theory.

However, The calculated result shows that Q1 is smaller than Q2. As mass flow rate grows smaller, the gap between Q1 and Q2 become greater. Even if I refined the mesh and set boundary layer of fluid, the gap still remains and becomes even larger.

I also check the heat from cooling plate internal surface to fluid Q3, which matches perfectly with Q1. So I guess there has to be issue of calculation of Q2.

I wonder if this is caused by numerical errors or by inappropriate models. The models I chose are:
segregated flow
k-epsilon turbulence model
segregated fluid temperature
conjugate heat transfer
I use surface average temperature of outlet boundary as Tout.

Can someone enlighten me why the gap exists? I'd be quite grateful.

FliegenderZirkus · April 25, 2022, 04:00

If the temperature profile at your inlet and outlet boundaries is not constant (which it typically won't be), you cannot use the "1D lumped" formula you wrote, but rather have to integrate local heat flux at each position at the surface $\dot{Q} =c_p \int_{A, outlet} \dot{m}TdA - c_p \int_{A, inlet} \dot{m}TdA$
It's not enough to use surface averages. Another factor is the heat conduction on the boundary which is calle "Flow Boundary Diffusion" in starccm+, when this is on, even the integrated formula won't give you exact heat balance. Usually it's best to just use the "heat transfer" report available in starccm+ which handles this automatically.
If this won't solve the imbalance, check if the case is truly converged. Solving the energy equation on solids can take many iterations with default URFs, often you can increase this to something like 0.999, but that's of course case specific.

tjushang · April 25, 2022, 09:27

Quote:

Originally Posted by FliegenderZirkus

If the temperature profile at your inlet and outlet boundaries is not constant (which it typically won't be), you cannot use the "1D lumped" formula you wrote, but rather have to integrate local heat flux at each position at the surface $\dot{Q} =c_p \int_{A, outlet} \dot{m}TdA - c_p \int_{A, inlet} \dot{m}TdA$
It's not enough to use surface averages. Another factor is the heat conduction on the boundary which is calle "Flow Boundary Diffusion" in starccm+, when this is on, even the integrated formula won't give you exact heat balance. Usually it's best to just use the "heat transfer" report available in starccm+ which handles this automatically.
If this won't solve the imbalance, check if the case is truly converged. Solving the energy equation on solids can take many iterations with default URFs, often you can increase this to something like 0.999, but that's of course case specific.

Thank you so much for your reply~
I totally agree with your idea and I tried to build a small zone near outlet and extract mass average temperature of this zone in order to rule out the effect of nonuniformity of outlet velocity. But I found that does not work well. Compared surface average temperature, the mass avergae temperatrue seems to overestimate Q2 more. Maybe I should check the other two reasons you raised.

FliegenderZirkus · April 25, 2022, 09:32

Why don't you just use the heat transfer report and select both inlet and outlet as the input parts? This way you should get the desired heat balance directly (one enthalpy will be positive, one negative, so you get a difference)

tjushang · April 25, 2022, 20:38

Quote:

Originally Posted by FliegenderZirkus

Why don't you just use the heat transfer report and select both inlet and outlet as the input parts? This way you should get the desired heat balance directly (one enthalpy will be positive, one negative, so you get a difference)

Thank you Zirkus. I tried this method and it shows perfect conservation of energy. I should have comprehended this heat transfer report earlier.

tjushang · April 26, 2022, 03:09

Quote:

Originally Posted by FliegenderZirkus

Why don't you just use the heat transfer report and select both inlet and outlet as the input parts? This way you should get the desired heat balance directly (one enthalpy will be positive, one negative, so you get a difference)

Hey guy, I just found that using "mass flow average" of inlet and outlet temperature may fit the 1D lump formula I wrote above. Thanks again.

April 25, 2022, 02:53	Inconsistency of heat transfer in steady state simulation using Star-CCM+	#1
tjushang New Member Yibao Shang Join Date: Jun 2014 Location: China Posts: 15 Rep Power: 11	Hi everyone, Recently I carried out a numerical simulation using Star-CCM+ which can be described as following: A cube is put on a cooling plate with rectangular channels. A total heat source of Q1 is set on the cube. The fluid inside rectangular has an inlet mass flow rate of m, inlet temperature of Tin, outlet temperature of Tout. The specific heat of fluid is represented as Cp. Thus the heat taken away by fluid can be calculated by *Q2 = Cp m * (Tout - Tin) in steady state. Other boundaries other than inlet and outlet are all set as adiabatic. If the described case reaches steady state, then Q1 = Q2 in theory. However, The calculated result shows that Q1 is smaller than Q2. As mass flow rate grows smaller, the gap between Q1 and Q2 become greater. Even if I refined the mesh and set boundary layer of fluid, the gap still remains and becomes even larger. I also check the heat from cooling plate internal surface to fluid Q3, which matches perfectly with Q1. So I guess there has to be issue of calculation of Q2. I wonder if this is caused by numerical errors or by inappropriate models. The models I chose are: segregated flow k-epsilon turbulence model segregated fluid temperature conjugate heat transfer I use surface average temperature of outlet boundary as Tout**. Can someone enlighten me why the gap exists? I'd be quite grateful.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Setting the height of the stream in the free channel	kevinmccartin	CFX	12	October 13, 2022 21:43
Continuity Equation for multicomponent simulation	lordluan	CFX	15	May 19, 2020 18:36
Compression stoke is giving higher pressure than calculated	nickjuana	CFX	62	May 19, 2015 13:32
Difficulty In Setting Boundary Conditions	Moinul Haque	CFX	4	November 25, 2014 17:30
star design - to model heat transfer	gagi	Main CFD Forum	0	November 11, 2011 01:41

April 25, 2022, 04:00		#2
FliegenderZirkus Member Join Date: Nov 2019 Posts: 93 Rep Power: 6	If the temperature profile at your inlet and outlet boundaries is not constant (which it typically won't be), you cannot use the "1D lumped" formula you wrote, but rather have to integrate local heat flux at each position at the surface $\dot{Q} =c_p \int_{A, outlet} \dot{m}TdA - c_p \int_{A, inlet} \dot{m}TdA$ It's not enough to use surface averages. Another factor is the heat conduction on the boundary which is calle "Flow Boundary Diffusion" in starccm+, when this is on, even the integrated formula won't give you exact heat balance. Usually it's best to just use the "heat transfer" report available in starccm+ which handles this automatically. If this won't solve the imbalance, check if the case is truly converged. Solving the energy equation on solids can take many iterations with default URFs, often you can increase this to something like 0.999, but that's of course case specific.

April 25, 2022, 09:32		#4
FliegenderZirkus Member Join Date: Nov 2019 Posts: 93 Rep Power: 6	Why don't you just use the heat transfer report and select both inlet and outlet as the input parts? This way you should get the desired heat balance directly (one enthalpy will be positive, one negative, so you get a difference)