Who knows how to print the results from CFX-4.2. Thanks

Hi, look at the bottom of this command file >>OUTPUT OPTIONS
>>PRINT OPTIONS >>WHAT pick what you want when you want it. Read Chapter 9. in the user guide (~page 159 in 1995 guide) that should tell you all you need to know. Good luck with CFX - you'll need it !! Regards James Date

>>CFX4
>>OPTIONS

THREE DIMENSIONS

BODY FITTED GRID

CARTESIAN COORDINATES

TURBULENT FLOW

ISOTHERMAL FLOW

INCOMPRESSIBLE FLOW

STEADY STATE
>>MODEL DATA
>>DIFFERENCING SCHEME

U VELOCITY 'UPWIND'

V VELOCITY 'UPWIND'

K 'UPWIND'

EPSILON 'UPWIND'
>>TITLE

PROBLEM TITLE 'BOUNDARY CONDITION STUDY'
>>PHYSICAL PROPERTIES

>>STANDARD FLUID

FLUID 'WATER'

STANDARD FLUID REFERENCE TEMPERATURE 2.7300E+02

>>TURBULENCE PARAMETERS

>>TURBULENCE MODEL

TURBULENCE MODEL 'K-EPSILON'
>>SOLVER DATA
>>PROGRAM CONTROL

MAXIMUM NUMBER OF ITERATIONS 1000

MAXIMUM CPU TIME 14400

OUTPUT MONITOR POSITION 5.000000E-01 5.000000E-01 5.000000E-01

MASS SOURCE TOLERANCE 1.0000E-06
>>EQUATION SOLVERS

U VELOCITY 'AMG'

V VELOCITY 'AMG'

PRESSURE 'AMG'

K 'AMG'

EPSILON 'AMG'
>>PRESSURE CORRECTION

PISO
>>UNDER RELAXATION FACTORS

U VELOCITY 7.5000E-01

V VELOCITY 7.5000E-01

PRESSURE 1.0000E+00

VISCOSITY 1.0000E+00

K 7.5000E-01

EPSILON 7.5000E-01
>>CREATE GRID
>>INPUT GRID

READ GRID FILE

FORMATTED
>>MODEL BOUNDARY CONDITIONS
>>PRESSURE BOUNDARIES

PATCH NAME 'FACE-NUMBER-0'

PRESSURE 0.0000E+00
>>PRESSURE BOUNDARIES

PATCH NAME 'FACE-NUMBER-36'

PRESSURE 0.0000E+00
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-3'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-8'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-13'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-18'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-23'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-28'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-33'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>SET VARIABLES

PATCH NAME 'FACE-NUMBER-37'

U VELOCITY 1.0000E+00

PRESSURE 0.0000E+00

K 1.0000E-03

EPSILON 1.0000E-03
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-6'
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-11'
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-16'
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-21'
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-26'
>>WALL BOUNDARY CONDITIONS

PATCH NAME 'FACE-NUMBER-31'
>>OUTPUT OPTIONS
>>PRINT OPTIONS

>>WHAT

U VELOCITY

V VELOCITY

W VELOCITY

PRESSURE

DENSITY

VISCOSITY

K

EPSILON

WALL PRINTING

>>WHERE

K PLANES 1

ALL BLOCKS

>>WHEN

INITIAL GUESS

FINAL SOLUTION

EACH TIME STEP

EACH ITERATION
>>STOP

Hello,

CFX produces a dump file with the results which can be viewed using graphical tools such as View and Visualize. If you want to extract results from the solution and output them to a text file, you can use the USRPRT subroutine.

This subroutine allows you to print out any variable at any time in the solution and at any place in the domain. I have used this to extract data along specific lines in the domain and use the data as the input for other simulations. It is the only way to automate post-processing.

I have posted a sample fortran file using this subroutine at:

http://bgtibm1.me.uiuc.edu/people/d-...lot/index.html

Please read the explanation of this subroutine; I just got it to the point where it did what I needed, and there are a few problems with it. It could be a VERY useful utility with some more work.

David Creech CFD Literature Catalog CFD Subroutine Archive

(1). I am surprised that one is still interested in printing out the results file. Back in early 70's, I used to get one big box of printout for every 3-D Navier-Stokes run. Since then, I have decided to save nature resources by using graphic post-processing. (2). For a 3-D case with a 250,000 mesh points, there will be 10 essential variables per mesh point ( x,y,z,u,v,w,p,t,rho,mu ). This is a minimum list, the total number of variables is 250,000 x 10 = 2,500,000. If we print 10 numbers per line, we have 250,000 lines of output. If one can print 80 lines per page using small font size, then we will have 250,000/80 = 3125 pages. This is equivalent to 4 thick books, each with 800 pages. (3). It is a good idea to do internal processing and save only needed results first, without printing or even file saving at all. ( I am constantly running out of disk space. And the solution is vey simple, just delete the files. ) (4). How long would it take to read 4 thick books of computed results? ( I had plotted 3-D results from printout to get velocity vector field plots with arrow heads included, once a long time ago. )

I have never found a need to print out the entire solution. What I have found very useful is the ability to print out single lines or planes of data. I do this in cases where I am interested in comparing line plots of some variable for large parametric studies. This is much faster than starting up a postprocessor, defining a line, and outputing the results to a file.

Another reason that I do this is when I am taking the output of a cfd solution (such as the heat flux at a wall) and use this as the input of another simulation (such as a custom code to predict steel shell solidification).

(1). Yes, I think the interface between codes is the place where interaction is always required. (2). And the graphic post-processing or inline-processing is essential to the future of CFD.