CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

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

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 25, 2022, 02:53
Default Inconsistency of heat transfer in steady state simulation using Star-CCM+
  #1
New Member
 
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10
tjushang is on a distinguished road
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.
tjushang is offline   Reply With Quote

Old   April 25, 2022, 04:00
Default
  #2
Member
 
Join Date: Nov 2019
Posts: 41
Rep Power: 4
FliegenderZirkus is on a distinguished road
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.
FliegenderZirkus is offline   Reply With Quote

Old   April 25, 2022, 09:27
Default
  #3
New Member
 
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10
tjushang is on a distinguished road
Quote:
Originally Posted by FliegenderZirkus View Post
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.
tjushang is offline   Reply With Quote

Old   April 25, 2022, 09:32
Default
  #4
Member
 
Join Date: Nov 2019
Posts: 41
Rep Power: 4
FliegenderZirkus is on a distinguished road
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)
FliegenderZirkus is offline   Reply With Quote

Old   April 25, 2022, 20:38
Default
  #5
New Member
 
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10
tjushang is on a distinguished road
Quote:
Originally Posted by FliegenderZirkus View Post
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 is offline   Reply With Quote

Old   April 26, 2022, 03:09
Default
  #6
New Member
 
Yibao Shang
Join Date: Jun 2014
Location: China
Posts: 15
Rep Power: 10
tjushang is on a distinguished road
Quote:
Originally Posted by FliegenderZirkus View Post
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.
tjushang is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 01:43.