|
[Sponsors] |
April 16, 2021, 10:47 |
Simulation heat transfer
|
#1 |
Member
Mercurial
Join Date: Mar 2021
Posts: 72
Rep Power: 5 |
Hi guys,
I'm trying to simulation the air through the reactangular duct which has 4 cylinder inside. My boundary condition is velocity inlet 9.45(Re=15000), pressure outlet =0, lower wall is heat wall, heat flux is changed from 500 to 5000. But when i changed heat flux, my result Nusselt number on heat wall and cylinder absolutely didn't change. Just temperature change. I don't know why. Please someone help me The second problem is when heat flux from 1000 to 5000, fluent notify " temperature limited to 1.000000e+00/5.00000e+003 in X cells on zone X" at the both first and second iteration . I searched in forum and they said because of grid. I use ICEM and qualify determinant 2x2x2 is around 0.9-1. y+<1 for using kw SST. Anyone met this problem before can help me understand ? Thanks all. |
|
April 16, 2021, 11:06 |
|
#2 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
If you change the heat flux and only see that only the temperature changes, this is absolutely correct! Heat transfer coefficient and Nusselt number is a property of the flow, it should not change with heat flux except due to non-linearities. By non-linearities, we mean that the heat flux changes the local fluid properties enough to change the flow. Otherwise, for relatively small changes in heat flux, the flow is unaffected and the Nusselt number should not change.
A better mesh always helps but if your solution converged for a heat flux of 1000 and only crashed when you changed the heat flux to 5000, then it can also just be an initialization problem. Have you tried using the converged solution with a heat flux of 1000 and then changing the heat flux instead of re-initializing? |
|
April 16, 2021, 11:54 |
|
#3 | |
Member
Mercurial
Join Date: Mar 2021
Posts: 72
Rep Power: 5 |
Quote:
About the error temperature limited, we are the same way. Because my document i using to simulation don't have the quality of heat flux, they just said that heat wall is assigned with constant heat flux so i'm finding the value consistent with their result. It's document from turbo expo 2019. u said try using the converged solution with heat flux 1000 and then changing the heat flux instead of re'initializing. I dont understand. why can i calculate if we don't re-initialize when heat flux change. I think it's wrong. Can u explain. Thanks |
||
April 16, 2021, 12:12 |
|
#4 | |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,400
Rep Power: 47 |
Quote:
What's most likely happening in your simulation: For the first few iterations, the fluid velocity near some parts of the heated wall is very low. Yet the boundary dumps a lot of heat into it. That can cause very high temperature in some of the cells near the heated wall. There are ways to fix this, like initializing the velocity field differently, lowering under-relaxation for energy equation, disabling energy altogether for the first few iterations etc. But if the simulation does not blow up, and continues to converge normally afterwards, you don't really have to do anything about it. |
||
April 16, 2021, 15:11 |
|
#5 | ||
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
Quote:
Quote:
If the warning goes away after some iterations that's fine too, that's normal. |
|||
May 7, 2021, 11:58 |
|
#6 |
New Member
Tamil Nadu
Join Date: Apr 2021
Posts: 6
Rep Power: 5 |
I am trying a case with a 2d rectangular channel having a supersonic flow (pressure inlet and pressure outlet boundary condition). The lower wall is set with a heat flux value of 5000W/m^2. Mine is a very simple case - compressible flow with heat addition. But the heat provided from the bottom wall does not have a noticeable effect on the flow. Can someone suggest an alternative method or explain my mistake.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Coupled Heat and Mass Transfer | Mecroob | OpenFOAM Running, Solving & CFD | 1 | July 12, 2020 19:24 |
Error - Solar absorber - Solar Thermal Radiation | MichaelK | CFX | 12 | September 1, 2016 05:15 |
New guy trying to solve his first simple Heat Transfer simulation. | BhaluBear | OpenFOAM | 2 | August 12, 2014 12:54 |
Setup of a turbine stator blade conjugate heat transfer simulation | mitra22 | CFX | 0 | February 7, 2014 04:53 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 15:55 |