# What are the 21 numbers in reactingFoam/constant/thermo.compressibleGas?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 24, 2011, 16:13 What are the 21 numbers in reactingFoam/constant/thermo.compressibleGas? #1 New Member   Scot Johnson Join Date: Mar 2011 Posts: 25 Rep Power: 8 Sponsored Links The reactingFoam tutorial is about combustion of methane, so in constant/thermo.compressibleGas is the list of reactants and products. Each one, such as O2, has 21 numbers associated with it. The second number is molecular weight, but what are the 20 others? I sure wish the user's guide had more. Thank you, very much indeed, for any help you can provide! Scot

 March 26, 2011, 15:11 #2 New Member   Valerio Novaresio Join Date: Mar 2009 Location: Polonghera, Cuneo, Italy Posts: 27 Rep Power: 10 Hi Scot, let me take the O2 like an example: O2 O2 1 31.9988 200 5000 1000 3.69758 0.00061352 -1.25884e-07 1.77528e-11 -1.13644e-15 -1233.93 3.18917 3.21294 0.00112749 -5.75615e-07 1.31388e-09 -8.76855e-13 -1005.25 6.03474 1.67212e-06 170.672 2° number -> molar weight (31.9988) 3° - 5° numbers -> temperature ranges where the interpolations are valid (min T = 200 K, max T = 5000 K, "middle" T = 1000 K. So we have two ranges: from 200 K to 1000 K and from 1000 K to 5000 K) 6° - 12° numbers -> seven coefficients for Janaff interpolation (cp, h, S) for the first temperature range (3.69758 0.00061352 -1.25884e-07 1.77528e-11 -1.13644e-15 -1233.93 3.18917) 12° - 19° numbers -> seven coefficients for Janaff interpolation (cp, h, S) for the second temperature range (3.21294 0.00112749 -5.75615e-07 1.31388e-09 -8.76855e-13 -1005.25 6.03474) 20° - 21° numbers -> coefficients for Sutherland interpolation for viscosity (1.67212e-06 170.672) Regards, Valerio mm.abdollahzadeh and wayne14 like this. __________________ ...The best way to acquire new knowledge is to share it...

 April 4, 2011, 09:43 #3 New Member   Scot Johnson Join Date: Mar 2011 Posts: 25 Rep Power: 8 Thank you, Valerio! Scot

 April 4, 2014, 08:47 coeff for Argon ? #4 Senior Member   Mieszko Młody Join Date: Mar 2009 Location: POLAND, USA Posts: 142 Rep Power: 10 Dear Foamers, Do you now any place I could find these values for Argon ? temperature range 87 - 400K ?

 April 4, 2014, 12:28 #5 New Member   Tom Join Date: Jun 2013 Posts: 26 Rep Power: 6 Hi ziemowitzima In the following links you can find some tables of Argon: http://www.nist.gov/data/PDFfiles/jpcrd363.pdf and http://contrails.iit.edu/DigitalColl...CTDR64-068.pdf If you want to know about the liquid phase check: http://encyclopedia.airliquide.com/encyclopedia.asp? There you can find properties of nitrogen, carbon, dioxide, argon, hydrogen and oxygen. Between those properties: Density & temperature calculation of the liquid phase, based on the pressure. Regards!

 April 5, 2014, 05:59 #6 Senior Member   Mieszko Młody Join Date: Mar 2009 Location: POLAND, USA Posts: 142 Rep Power: 10 Thank you !

 October 1, 2014, 09:27 get the thermo data #7 New Member   Stratos Join Date: Aug 2014 Location: England Posts: 5 Rep Power: 5 Hi, Does anybody know how to retrieve the data in thermo.CompressibleGas from code? Reactingfoam code defines this object: Code: `psiReactionThermo& thermo = reaction->thermo();` as well as: Code: `basicMultiComponentMixture& composition = thermo.composition();` Both of them have valuable information butI cannot see how to get these values from these objects. One way could be to read the whole dictionary but this is not the most efficient way. Any ideas? Thanks

 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 ploceus OpenFOAM Running, Solving & CFD 6 June 15, 2009 04:00 Soheyl ANSYS Meshing & Geometry 0 May 25, 2009 20:38 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 maoasis FLUENT 0 April 24, 2006 10:51 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07