Hi, guys!

I write a batch run file as followed. Where the ccl files varies only from the TM.

__________________________________________________ _________

cfx5solve -batch -def *.def -part 2 -start-method "MPICH Local Parallel for Windows" -bg-ccl epsilon.ccl -name epsilon

cfx5solve -batch -def *.def -part 2 -start-method "MPICH Local Parallel for Windows" -bg-ccl omega.ccl -name omega

__________________________________________________ _________

The first run goes on well and get a good result. But the second one was interrupted by the following error. I don't understand the meaning of "signal HUP(1)". Please help me.

Jia

__________________________________________________ _________

Error detected by routine MAKDAT CDANAM = ICTYPE CDTYPE = CHAR ISIZE = 12 CRESLT = OLD

Current Directory : /FLOW/INITCON/ZN1/VARIABLES/TED_FL1 STOP called from routine MEMERR +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | C:\Program Files\Ansys Inc\v110\CFX\bin\winnt\cclsetup.exe was | | interrupted by signal HUP (1) | +--------------------------------------------------------------------+

/FLOW/INITCON/ZN1/VARIABLES/TED_FL1

INITCON is for initial conditions ZN1 means first domain (but not necessarily in your order) TED_FL1 means Turbulence Eddy Dissipation for first Fluid

So there is a problem with the initialisation of turbulence eddy dissipation in one of your domains.

MAKDAT CDANAM = ICTYPE CDTYPE = CHAR ISIZE = 12 CRESLT = OLD

MAKDAT means the solver wants to MAKe a DATa area with name ICTYPE and type CHARacter with length 12, but found that this was already there (CRESLT=OLD).

So check your CCL for double entries regarding the initialisation of turbulence eddy dissipation.

Good luck!

Hi,Andreas!

Thanks very much! Your explain is exactly and in time. At the same time, I read the help on subroutine MAKDAT. It also helps a lot.

However, I have change the initialisation of TED in ccl file as attached. The error still emerged.

By the way, if running by GUI model with the exactly same settings, the error has never happened. Do you have further suggestions? Thanks!

Jia

__________________________________________________ _________

INITIALISATION:

Option = Automatic

INITIAL CONDITIONS:

Velocity Type = Cartesian

CARTESIAN VELOCITY COMPONENTS:

Option = Automatic with Value

U = 20 [m s^-1]

V = 0.2 [m s^-1]

W = 0 [m s^-1]

END

K:

Option = Automatic with Value

k = 0.0004 [m^2 s^-2]

END

OMEGA:

Eddy Length Scale = 18 [mm]

Epsilon = 0.0004 [m^2 s^-3]

Option = Automatic with Value

END

STATIC PRESSURE:

Option = Automatic with Value

Relative Pressure = 1 [atm]

END

TEMPERATURE:

Option = Automatic with Value

Temperature = 310 [K]

END

END END

__________________________________________________ _________

Are you sure you wanted to use -bg-ccl and not -ccl, i.e. using your ccl as default and not as override? You should check the out file whether there are initialisation entries that are contradicting. Not the whole INITIALISATION singleton is replaced so that entries from the def file will be also there and this may cause problems.

[Saima]

Hi ,

I am doing CFX in bact mode by using command:

C:\Users\sanaz\Desktop>"C:\Program Files\ANSYS Inc\v121\CFX\bin\cfx5pre.exe" -batch ROTOR.pre -icem project.msh

and i am getting error:
- Unable to read the "Length Units" from the "SOLVER UNITS" object.

Kindly let me know how can i avoid it. I dont understand about it.

Regards,

[ghorrocks]

Exactly what it says - there is an error in setting the length units. Have a look at the batch file script.

[Saima]

Originally Posted by ghorrocks

Exactly what it says - there is an error in setting the length units. Have a look at the batch file script.

Yes, you are right, i solved it.

But now i got error in runing def file.

I am using command:
C:\Users\sanaz\Desktop>"C:\Program Files\ANSYS Inc\v121\CFX\bin\cfx5solve" -def Rotor_67.def

It produce my result file but it also give the messgae:

"Feature CFX_SOLVER_BASIC_MP_LIMIT does not exist in the ANSYSLI pool."

Acutally i mam using batch mode in iSIGHT optimization software this software stop after getting this messgae it takes as an error.

[ghorrocks]

That is a licensing problem. Check you have the necessary licenses to run your model.