
[Sponsors] 
Inconsistency of heat transfer in steady state simulation using StarCCM+ 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 25, 2022, 02:53 
Inconsistency of heat transfer in steady state simulation using StarCCM+

#1 
New Member
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10 
Hi everyone,
Recently I carried out a numerical simulation using StarCCM+ 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 kepsilon 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. 

April 25, 2022, 04:00 

#2 
Member
Join Date: Nov 2019
Posts: 41
Rep Power: 4 
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
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, 09:27 

#3 
New Member
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10 
Quote:
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. 

April 25, 2022, 09:32 

#4 
Member
Join Date: Nov 2019
Posts: 41
Rep Power: 4 
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)


April 25, 2022, 20:38 

#5 
New Member
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10 
Thank you Zirkus. I tried this method and it shows perfect conservation of energy. I should have comprehended this heat transfer report earlier.


April 26, 2022, 03:09 

#6 
New Member
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10 
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.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Continuity Equation for multicomponent simulation  lordluan  CFX  15  May 19, 2020 18:36 
Setting the height of the stream in the free channel  kevinmccartin  CFX  10  July 9, 2015 21:36 
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 