[.bastian]

Hello.

Right now i'm trying to define own material properties in Ansys CFX (R19) using the value option and equations depending on pressure and temperature.

For example my equation for specific heat at constant pressure is looking like this:

(4.105976721700E+003+1.061520419350E-005*(p*1 [Pa^-1])+8.513734104789E-012*((p*1 [Pa^-1])^2)-1.838534834997E-016*((p*1 [Pa^-1])^3)-5.325809123258E+000*(T*1 [K^-1])-1.002737641102E-007*(T*1 [K^-1])*(p*1 [Pa^-1])+1.632147648588E-007*(T*1 [K^-1])*((p*1 [Pa^-1])^2)-1.573807426520E-024*(T*1 [K^-1])*((p*1 [Pa^-1])^3)+2.284578823171E-002*((T*1 [K^-1])^2)+3.118097032835E-010*((T*1 [K^-1])^2)*(p*1 [Pa^-1])-1.966729989433E-019*((T*1 [K^-1])^2)*((p*1 [Pa^-1])^2)+1.430074218860E-017*((T*1 [K^-1])^2)*((p*1 [Pa^-1])^3)-2.428562434427E-005*((T*1 [K^-1])^3)-3.229774746216E-013*((T*1 [K^-1])^3)*(p*1 [Pa^-1])+3.663732513675E-012*((T*1 [K^-1])^3)*((p*1 [Pa^-1])^2)+1.181683926195E-029*((T*1 [K^-1])^3)*((p*1 [Pa^-1])^3)) [J kg^-1 K^-1]

All other equations are of similar shape with sometimes lower or higher polinomial degrees.

Now when i apply the material to my model the solver crashes while initializing showing:

  Fatal bounds error detected
  ---------------------------
  Variable: Specific Heat Capacity at Constant Pressure
  Locale  : 

 +--------------------------------------------------------------------+
 |                    Writing crash recovery file                     |
 +--------------------------------------------------------------------+
  
 Details of error:-
 ----------------
 Error detected by routine MAKDAT 
 CDANAM =  LVAR CDTYPE =  INTR ISIZE =  136
 CRESLT = OLD 
  
 Current Directory : /FLOW/ALGORITHM/ZN1/SYSTEM/VARIABLES

 +--------------------------------------------------------------------+
 |                An error has occurred in cfx5solve:                 |
 |                                                                    |
 | The ANSYS CFX solver exited with return code 1.   No results file  |
 | has been created.                                                  |
 +--------------------------------------------------------------------+

End of solution stage.

With any suitable standard material a solution is generated without any problem.

My first attempts to solve this problem on my own where going from an arbitrary constant value for the heat capacity to more complex polynomials.
In this regard i figured out that this:

(3900-0.01*T*1[K^-1])[J kg^-1 K^-1]

worked without any problems, while changing it to a term of higher power:

(3900-0.01*(T*1[K^-1])^2)[J kg^-1 K^-1]

or also

(3900-0.01*T^2*1[K^-2])[J kg^-1 K^-1]

is leading to the described crash.

Maybe someone of you can give me a hint what i am doing wrong with the higher term dependencies. Right now im running out of ideas to solve this problem.

Thanks in advance!

bastian.

[ghorrocks]

CFX uses your functions to generate a table of values, and it uses that table of values in the simulation. The table has user settable maximum and minimum values and your function looks like it goes haywire as it approaches the maximum and minimum values.

So I recommend you look at the table generation settings in the materials tab. Set the maximum and minimum values to cover the range expected in your simulation. You will find the default values are very wide.

[.bastian]

Hello ghorrocks,

at first thank you for your answer.

That was also one of my first attempts before i tried switching to the described stepwise expansion of the polinomial.

But also with an appropriate range in pressure and temperature (cf. picture below) and several tries changing the the maximum points or switching on/off the extrapolation settings it ends in the described error.

Leaving the first (full) equation beside im curious about that the simple attempt with T^1 runs without any problems while the simple change to the next higher polynomial T^2 leads into the error.

Its driving me nuts..

[Opaque]

Material properties are not for the faint of the heart. It requires a lot of patience and being aware of the thermodynamic requirements.

Noticed your specific heat capacity is a function of pressure. Do you have a consistent set of properties? Cp has a strong relationship with the equation of state, i.e. rho(T,p). Have you read the documentation section

CFX-Solver Theory Guide/Chapter 1: Basic Solver Capability Theory | 1.2. Governing Equations/Equation of State/General Equation of State

If your equations are not thermodynamically consistent, the generation of the tables is nearly impossible. You may manage to create one by reducing the tolerances, but you will be pushing the problem downstream during the solution of the discrete equations. The model may never converge, since it cannot satisfy thermodynamics, regardless of timestep or any trick to force it to do so.

In your simple case, Cp = f(T^2), is the set of properties consistent? are the table generation controls appropriate for the integration in the solution range you expect the iterative process to occur?

Hope the above helps

[.bastian]

Thank you for your reply.

In fact i didn't know that there has to be an exact consistency between cp and rho which exactly seems to be the key to my problem.

Against the background of my project i need properties for a cooling fluid containing water and mono-ethylene-glycol (mixture: 80/20).
So i used a curve fitting algorithm to get equations for the particular properties on base of tabulated values generated with Refprop.

Therefore there is surely no exact thermodynamic consistency between the individual equations.

I would say - lesson learned , i have to search for another approach.
Thanks for your kind help guys.