[mhsr]

I defined a simulation in CFX 12.0.1 including an outlet condition with mass and momentum options 'Average Static Pressure' and 'Circumferential' as type of the pressure profile at the boundary face. Since the face is not centered on any global axis I defined a local coordinate system at the centroid of the outlet face in CFX-Pre. The z axis of this coordinate system is used as axis for the bands of the pressure profile.

The solver (on amd64 platform) runs fine until any (intermediate) results are to be written. The solver run finishes with following error message:

Error detected by routine PEEKI
CDANAM=/FLOW/GETVAR/GEOM_DIR/KZifBcp
CRESLT=NONE
Current Directory = /FLOW/SOLUTION/TSTEP328/CLOOP1/ZN1/BELG1/IP

Same error occurs when using the parallel global Z axis or a 'two point'-axis.

I also checked it with option 'Average Over Whole Outlet' which gave no errors.

Can anyone confirm that problem?

[Katha]

Hello, old thread but nevertheless. I am getting a similar error while trying to use a static pressure profile as outlet boundary condition. Running the same simulation with average static pressure at the outlet did not lead to any errors.
Has anyone had experience using profile boundary conditions at the outlet?
My exact error is:
Details of error:-
----------------
Error detected by routine PEEKR
CDANAM = PRAV/VALUE
CRESLT = NONE

Current Directory : /FLOW/BOUNDCON/ZN1/BCP5/VARIABLES
　
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+
S ave: 48
+--------------------------------------------------------------------+
| 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.

Thanks for any replies.

[Opaque]

Which version of ANSYS CFX are you using?

Would you mind posting the command input file section for the OUTLET boundary only?

[Katha]

sure. so I am using V16.2. I am not exactly sure about your second request. So my input .csv file looks like this:
(I used:: File --> Export with the settings: Type --> BC Profile, Locations --> "Myoutlet", Boundary Data --> Current, Profile Type --> Outlet Pressure)

[Name]
outlet
　
[Spatial Fields]
x, y, z
　
[Data]
x [ m ], y [ m ], z [ m ], Pressure [ Pa ]
1.30634427e-01, -1.85960054e-01, 7.78903842e-01, 9.71218906e+04
1.30705997e-01, -1.85479924e-01, 7.76850283e-01, 9.70624375e+04
1.34083450e-01, -1.84209853e-01, 7.77318776e-01, 9.64650781e+04
1.34233251e-01, -1.84557319e-01, 7.79178202e-01, 9.63172422e+04
.
.
.
And this is how I use it as BC profile in CFX Pre:

LIBRARY:
CEL:
&replace FUNCTION: outlet
Argument Units = [m], [m], [m]
File Name = /users/........../exportOut.csv
Option = Profile Data
Profile Function = On
Render Type = Points
Spatial Fields = x, y, z
DATA FIELD: Pressure
Field Name = Pressure
Parameter List = Pressure Profile Shape,Relative Pressure,Relative Pressure in Gas,Relative Static Pressure,Relative Total Pressure
Result Units = [Pa]
END
END
END
END

I am not sure whether this is, what you needed to see.
Also its probably worth mentioning, that I am also using a total pressure Profile at the inlet which works without issues.

[Katha]

I found the issue. So as I said I had been using an average static pressure boundary condition before and wanted to switch to the static pressure profile. Therefore I initialised the outlet profile and used the tickbox "Use Profile Data" in the Setup of the according BC. i did not realize, that in the boundary details it would keep up the Average Pressure settings. This seemed to have been the problem. Now, that I changed the Option in "Mass and Momentum" to "Static Pressure" (the logical option) I do not get the same error again.