|
[Sponsors] |
October 1, 2013, 14:02 |
CFX vs Icepak
|
#1 |
New Member
Join Date: Oct 2013
Posts: 9
Rep Power: 12 |
Hi,
I am new to CFX and I'm running a conjugate heat transfer problem in CFX which has already been run in Icepak. Sadly I am not getting the same result as that got in Icepak. I have around 70-80 degree C temperature variation on my bodies. Could anyone please tell common reasons for the change in results? or if it is not anything unusual to get varied results (due to different solver,etc. ) Thanks |
|
October 1, 2013, 15:01 |
|
#2 |
Member
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 50
Rep Power: 13 |
I don't know Icepak but I' am currently doing some CHT studies with CFX.
Would be helpful for us, if you told us some details about your setup. What are your y+ values? What turbulence model are you using? |
|
October 1, 2013, 16:51 |
|
#3 |
New Member
Join Date: Oct 2013
Posts: 9
Rep Power: 12 |
Thanks for the reply. I am not sure what you mean by y+ values and I use High intensity turbulence.
|
|
October 1, 2013, 20:39 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
||
October 2, 2013, 05:00 |
|
#5 |
Member
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 50
Rep Power: 13 |
Y+ is the dimensionless wall distance. It is used as an argument in wall functions (WF). Dependent from the turbulence model and mesh resolution WF are used to calculate the velocity and temperature profile in the boundary layer (BL). As they model the BL based on physical assumptions, they are only an approximation for the real values inside th BL.
Okay you have high intensity turbulence, but what turbulence model are you using? Go to your Fluid Domain in the CFX-Pre Outline and edit it. Under Fluid Models/Turbulence you can find the turbulende model. |
|
October 2, 2013, 11:45 |
|
#6 |
New Member
Join Date: Oct 2013
Posts: 9
Rep Power: 12 |
Hi ghorrocks,
Thanks for the link! |
|
October 2, 2013, 11:51 |
|
#7 |
New Member
Join Date: Oct 2013
Posts: 9
Rep Power: 12 |
Hi Daniel C,
I'm using the k-epsilon model and I have also tried using other models. Here is the simulation I'm trying to do; Heat transfer from a series of pipes which is hot (defined by a particular temperature, due to hot fluid flowing in it). This has been done in Icepak and now when I do it on CFX i get different results. However, when I increase the velocity in CFX to around 5 m/s (in icepak it is .5 m/s) then my temperature comes to be equal to what i get in Icepak. So, I was wondering if there is a problem with defining the turbulence in CFX that I am unable to crack. Thanks for reviewing the problem. |
|
October 3, 2013, 14:27 |
|
#8 | |
Member
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 50
Rep Power: 13 |
Quote:
And anyway, what makes you sure that the Icepak simulation is accurate? The heat Transfer is influenced by the flow conditions (laminar, turbulent) and the thermal boundary layer. For forced convection it is in general a relation of Re,Pr and Ec, thus Nu = f(Re,Pr,Ec). So you should keep the original Re number.The Eckert number Ec is not important as long as you have a lowspeed problem or when dissipation is negligible relatively to the forced convection. If your fluids Prandtl number Pr is around 1, then your thermal boundary layer has the same dimension as your flow boundary layer (BL). Make sure that your mesh either fully resolves the boundary layer, that means y+ < 1 or put enough points inside the BL appropiate for the turbulence model you are using. For the k-Epsilon turbulence model with Scaleable Wall Functions you can use a relatively coarse mesh with y+ >= 30. The k-w-SST model has Automatic Wall Treatment and you should put at least 15 Points into the BL. Also see http://www.cfd-online.com/Forums/cfx...lence-cfx.html for more information. But before you experiment with different turbulence models, you should perform a mesh independence study to ensure your solution doesn't vary with the mesh density. Good luck! |
||
October 7, 2013, 21:07 |
|
#9 |
New Member
Join Date: Oct 2013
Posts: 9
Rep Power: 12 |
ThankYou Sir for the help. I got the simulation running and giving correct results. But now there is a new problem. I have a change in the mesh that gives me results that vary by 20degree C at a particular point. Is that common?
|
|
October 7, 2013, 21:49 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
It certainly is common. You did not read the link I posted in post #4, did you?
The most common source of inaccuracy reported in the forum eventually turns out to be inadequate mesh resolution. You need to do a mesh sensitivity study to determine how fine a mesh you need for the accuracy you require. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
CFX Treatment of Laminar and Turbulent Flows | Jade M | CFX | 18 | September 15, 2022 07:08 |
High Resolution (CFX) vs 2nd Order Upwind (Fluent) | gravis | ANSYS | 3 | March 24, 2011 02:43 |
CFX pressure in Simulations problem | nasdak | CFX | 1 | April 14, 2010 13:22 |
PhD using CFX | Rui | CFX | 9 | May 28, 2007 05:59 |
FSI using CFX and ANSYS | Bi Chang | CFX | 2 | May 10, 2005 04:47 |