CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

CFX vs Icepak

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 1, 2013, 14:02
Default CFX vs Icepak
  #1
New Member
 
Join Date: Oct 2013
Posts: 9
Rep Power: 5
dren is on a distinguished road
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
dren is offline   Reply With Quote

Old   October 1, 2013, 15:01
Default
  #2
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 6
Daniel C is on a distinguished road
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?
Daniel C is offline   Reply With Quote

Old   October 1, 2013, 16:51
Default
  #3
New Member
 
Join Date: Oct 2013
Posts: 9
Rep Power: 5
dren is on a distinguished road
Thanks for the reply. I am not sure what you mean by y+ values and I use High intensity turbulence.
dren is offline   Reply With Quote

Old   October 1, 2013, 20:39
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   October 2, 2013, 05:00
Default
  #5
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 6
Daniel C is on a distinguished road
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.
Daniel C is offline   Reply With Quote

Old   October 2, 2013, 11:45
Default
  #6
New Member
 
Join Date: Oct 2013
Posts: 9
Rep Power: 5
dren is on a distinguished road
Hi ghorrocks,

Thanks for the link!
dren is offline   Reply With Quote

Old   October 2, 2013, 11:51
Default
  #7
New Member
 
Join Date: Oct 2013
Posts: 9
Rep Power: 5
dren is on a distinguished road
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.
dren is offline   Reply With Quote

Old   October 3, 2013, 14:27
Default
  #8
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 6
Daniel C is on a distinguished road
Quote:
Originally Posted by dren View Post
Hi Daniel C,
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.
Then you are comparing two different flow conditions. You know that increasing the velocity by a factor of 10 gives you a Re number that is ten times higher?

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!
Daniel C is offline   Reply With Quote

Old   October 7, 2013, 21:07
Default
  #9
New Member
 
Join Date: Oct 2013
Posts: 9
Rep Power: 5
dren is on a distinguished road
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?
dren is offline   Reply With Quote

Old   October 7, 2013, 21:49
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CFX Treatment of Laminar and Turbulent Flows Jade M CFX 14 June 15, 2016 09:36
High Resolution (CFX) vs 2nd Order Upwind (Fluent) gravis ANSYS 3 March 24, 2011 03:43
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


All times are GMT -4. The time now is 01:32.