# air varible property

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

 February 24, 2012, 08:50 air varible property #1 Member   Join Date: Aug 2011 Posts: 53 Rep Power: 7 Hello I am trying to simulate forced convection (air) where the film temperature is high enough to cause property variation in air. how can i make the thermal conductivity and viscosity of air, change wrt temperature? if CEL is the only way, may i have the general expression for K and wrt to temperature?

 February 25, 2012, 01:15 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 577 Rep Power: 11 an example of temperature dependent thermal conductivity would be: 0.002[W*m^-1*K^-3]*T^2+0.001[W*m^-1*K^-2]*T+0.1[W*m^-1*K^-1]

 February 25, 2012, 06:52 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 You can define properties as either CEL expressions or tables of values. Properties of air at various conditions are pretty easy to get with google.

 February 25, 2012, 10:46 #4 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 577 Rep Power: 11 You can also try getting NIST RefProp for fluid properties. Its free to students (only has water, air, and a few others). For only a small price you can buy their full package which has just about every fluid and property at any condition you can imagine.

 February 27, 2012, 04:19 #5 Member   Join Date: Aug 2011 Posts: 53 Rep Power: 7 hi, i get the following error when i try to run my code with CEL ---------------------------------------------------------------------------------- Fatal bounds error detected --------------------------- Variable: Thermal Conductivity Locale : air +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Stopped in routine ENFORCE_BOUNDS | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. | | | | It gave the following output: | | | | Contents of /tmp/pvml.504: | | | | [t80040000] 02/27 13:41:03 agni3 (10.1.8.3:43060) LINUXX86_64 3- | | .4.4 | | [t80040000] 02/27 13:41:03 ready Mon Feb 27 13:41:03 2012 | | No results file has been created. | +--------------------------------------------------------------------+ End of solution stage. ---------------------------------------------------------------------------------- my expression for Kth is : -------------------------------------------------------------------------------------(( - 2*10^(-14))[W/m/K^6)]*T^(5) ) + (( 1*10^(-11))[W*m^-1*K^-5]*T^(4) ) - ( (6*10^(-09))[W*m^-1*K^-4]*T^(3) ) + ( (1*10^(-06))[W*m^-1*K^-3]*T^(2) ) - (( 6*10^(-05))[W*m^-1*K^-2]*T ) + 0.006[W*m^-1*K^-1] ------------------------------------------------------------------------------------- If i need to define it as a reference table, how do i do it? pl. do reply asap thanks

 February 27, 2012, 06:05 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 Variable properties are always harder to converge. But the problem with using fitted equations like you have (which includes temperature up to the fifth power) is that outside of the fitted range the equations frequently go bezerk and lead to rapid divergence. A table can help here, at least they are better behaved out of the defined region. Use a 1D interpolation function and enter the points in. I usually do it by entering in a few points then editting the CCL of the interpolation function and add all the other points in a text editor. It is much easier to add lots of points in the text editor than the GUI.

 February 27, 2012, 06:33 #7 Senior Member   Join Date: May 2011 Location: Germany Posts: 130 Rep Power: 7 You can also use the sutherland-law for thermal conductivity and viscosity. This work quite fine for me in the past.

 February 27, 2012, 07:11 #8 Member   Join Date: Aug 2011 Posts: 53 Rep Power: 7 Hello all, thanks for the reply. Zigainer, The case is running with sutherlands formula. ghorrocks, cud u pl. explain me how to give an input as a table? May be i am not able to follow the steps explained. Regards

February 27, 2012, 07:41
#9
Senior Member

Join Date: May 2011
Location: Germany
Posts: 130
Rep Power: 7
Quote:
 Originally Posted by Studentdrak Zigainer, The case is running with sutherlands formula.
Did you use the pre-implemented sutherland formual or did you just created a new expression? Don't know if it makes any differences ....

 February 27, 2012, 17:50 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 If you want to use the interpolation function approach have a look it up in the documentation. It is quite easy to use.

 February 27, 2012, 23:34 #11 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 577 Rep Power: 11 Thermal conductivity is usually fit well by a second order curve fit. What crazy temperature range are you using to need a 5th order?? More importantly, and the reason its failing is: If you want to use such high order polynomials you have to include much more than one significant figure for your values. They become very important in the higher orders. Increase the sig figs in your curve fit values to as many as you can.

 February 28, 2012, 08:38 #12 Member   Join Date: Aug 2011 Posts: 53 Rep Power: 7 Thank u all Zigainer, i had used inbuilt sutherlands formula

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Issa CFX 3 November 23, 2009 18:16 saii CFX 2 September 18, 2009 08:07 xujjun CFX 9 June 9, 2009 07:59 Carl CFX 1 September 25, 2006 09:48 kim FLUENT 4 June 9, 2003 07:04

All times are GMT -4. The time now is 11:17.