CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   CFX vs Icepak (http://www.cfd-online.com/Forums/cfx/124301-cfx-vs-icepak.html)

dren October 1, 2013 14:02

CFX vs Icepak
 
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

Daniel C October 1, 2013 15:01

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?

dren October 1, 2013 16:51

Thanks for the reply. I am not sure what you mean by y+ values and I use High intensity turbulence.

ghorrocks October 1, 2013 20:39

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Daniel C October 2, 2013 05:00

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.

dren October 2, 2013 11:45

Hi ghorrocks,

Thanks for the link!

dren October 2, 2013 11:51

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.

Daniel C October 3, 2013 14:27

Quote:

Originally Posted by dren (Post 454725)
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!

dren October 7, 2013 21:07

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?

ghorrocks October 7, 2013 21:49

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.


All times are GMT -4. The time now is 15:34.