• CFD, Fluid Flow, FEA, Heat/Mass Transfer

Scripting Languages

Automation

Scripts, Journals, UDF, Field Functions

A collection of scripts, journals and macros in CFD simulations to automate some tasks as well as enhance simulation capabilities. One may need such functions to apply special boundary conditions such as inlet velocity which is function of both time and space. Scripts or macros can be used to repeat the same simulation with changed boundary conditions or can be used to create a checking log where the summary of boundary conditions, solver setting, material properties and interface/periodicity information can be written out in a log file for self and peer review.


Definitions and concepts
  • A STAR-CCM+ macro is a Java program that is compiled and executed within the STAR-CCM+ workspace. A FLUENT UDF is a C program that is compiled and executed within the FLUENT workspace.
  • CFX uses a high level programming called CCL or CFX command language. Unlike UDF or JAVA macros, it does not need to be interpreted or compiled. However, for special post processing, commands in PERL and accessing solver program in FORTRAN is required.
  • Note that specific heat capacity Cp cannot be accessed or changed via UDF in FLUENT.

Programs and Scripting/Macro Language
ICEM CFD STAR-CCM+ FLUENT CFX OpenFOAM ParaView ANSA HyperMesh
Tck/Tk Java SCHEME, C CCL, PERL, FORTRAN C++ Python Python Tcl/Tk

A sophisticated automation approach requires developement of a consistent naming convention for the geometry, surface, boundaries and volumetric regions (domains). This include CAD package, the pre-processor, solve and post-processor. Even the structure of CAD program (such as model tree) to represent an assembly need to be simple and consistent with CFD pre-processor. It may be an uphill task if the CAD program, the pre-processors and solvers uses different programming and scripting languages. For example, ANSYS SpaceClaim uses Python, FLUENT is based on SCHEME and the syntax in CFD-Post is CEL/PERL. In such cases, end-to-end automation may not yield desired advantages and a separate automation should be worked out at each step. FLUENT GUI is based on Qt Toolkit and graphical attributes can be modified using Qt stylesheets such as cxdisplay.css for FLUENT. This file needs to be placed in home directory (location where FLUENT executables are placed during installation). This article "Scripted CFD simulations and postprocessing in Fluent and ParaVIEW" by Lukas Muttenthaler et al at Johannes Kepler University Linz provides a detailed automation method which can be improvised further.

  • A guide describing syntax used in SCHEME language can be found here (Scheme programming).
  • Another book: Concrete Abstractions - An Introduction to Computer Science Using Scheme by Hailperin et al. can be found here. Some example from this book is provided towards end of this page.
  • A summary of few basic yet key features of the programming languages mentioned above is tabulated below.
  • SCHEME is a dialect of LISP (having fully parenthesised syntax) and is the second-oldest high-level programming language after FORTRAN. The command and variable names are case-insensitive (though should only contain small letters in ANSYS FLUENT).
  • Note: if in future ANSYS decides to re-write FLUENT GUI and TUI in some other programmins langauge say C++ or Python, the scripts described on this page may get obsolete.
  • ANSYS has a feature ACT to facilitate automation an customization of simulation workflows.
Feature Tcl/Tk FORTRAN C JAVA
Case-sensitive Y N Y Y
Comment # C, ! /* ... */ //
End of Statement ; Newline character ; ;
Line Continuation \ Any character \ Not required
Variable Definition set x = 1; real x = 1 real x = 1; real x = 1;
If Loop if { x == y } {
 x = x + 1;
}
if (x .EQ. y) then
 x = x + 1
endif
if (x = y) {
 x = x + 1;
}
if (x = y) {
 x = x + 1;
}
For Loop for {set j 1} {$j <= $n} {incr j} {
  ...
}
DO Loop for (i=0; i<= 10, i++) {
 ...
}
for (i=0; i<= 10, i++)
{
 ...
}
Arrays $x(5); x(5) x[5]; x[5];
File Embedding source "common.dat"; include "common.dat" #include "common.h"; import common.class;
Note:

Java doesn't need a "line continuation character" since the end of the line has no significance so long a semi-colon is added at the end of a statement. It acts just as any other whitespace character. In other words, one can end the line immediately after an x = and continue on the assignment (say 10 in x = 10) on next line without any problems. For Tck/Tk used in ICEM CFD, the end of statement is also a newline character. However, if more than one statements are to be put on a line, they can be separated by a semi-colon. In SCHEME, a string literal is continued from one line to another, the string will contain the newline character (#\newline) at the line break. Like most of the programming languages: string is written as a sequence of characters enclosed within double quotes " ". To include a double quote inside a string, precede the double quote with a backslash \ (escape it).


CFX uses PERL for automation such as for-loop and lists. It does not accept underscore or hyphen in names, though spaces are allowed.


Examples: In FLUENT, the in-built macros used to access components of the velocity are
  • C_U(c,t): x-component of velocity
  • C_V(c,t): y-component of velocity
  • C_W(c,t): z-component of velocity
In STAR-CCM, it is achieved as:
  • Magnitude: mag($$Velocity)
  • X-component: $$Velocity[1]
  • Y-Component: $$Velocity[1]...
  • The directions X,Y,Z are represented by [0],[1],[2] respectively.

An example of a journal script which can be used in FLUENT to set-up a solver is as follows. This journal just needs to be edited for user's need. Note that there should be no empty line till the end of file. An empty line is assumed to be end of input. Use the remark character ; instead. The journal can be further parametrized by defining parameter using syntax (define X 0.7). Similarly, mathematical operation can be performed e.g. a = a + 0.1 can be written as (define a (+ a 0.1)).

Script and Macros

(ti-menu-load-string) is used to invoke a TUI command in SCHEME journal i.e. to convert a journal command to Scheme command. e.g. (ti-menu-load-string "solve set time-step 0.01"). Return value: #t if successful, #f if error occurs or cancelled by pressing Ctrl-C. Note all the SCHEME commands should be inside parentheses ( ... ).


Example scripts to make batch runs: SINGLE PHASE

Steady State Cold Flow SIMPLE Gravity OFF Energy OFF
Steady State Cold Flow Coupled Psuedo-Transient Gravity OFF Energy OFF
Steady State Cold Flow Coupled Gravity OFF Energy OFF
Steady State Conjugate Heat Transfer SIMPLE Gravity OFF Energy ON
Steady State Conjugate Heat Transfer Coupled Psuedo-Transient Gravity OFF Energy ON

Terminate or Save and Terminate a FLUENT job running in batch-mode on remote server (cluter): GUI based method is to use "Remote Visualization Client". Another option is to create checkpoints in the script: e.g. (set! checkpoint/exit-filename "/FOLDER/exit-fluent-FILENAME") where 'FOLDER' is location to store the case and data files. FILENAME is some which needs to be created whenever you want to save the data: touch /FOLDER/exit-fluent-FILENAME


 (define rf 0.7)
  file/read-case fluent.msh
  ;
  ;Change solid-domains into fluid type
  define/boundary-conditions/modify-zones/zone-type 4 fluid
  ;
  mesh/repair-improve/allow-repair-at-boundaries y
  mesh/repair-improve/repair
  ;Check and reorder the mesh to reduce the bandwidth of matrix
  mesh/check
  mesh/mesh-info 0
  mesh/reorder/reorder-domain
  mesh/reorder/reorder-domain
  ;
  /file/set-batch-options no yes yes no
  (set! *cx-exit-on-error* #t)
  define/models/solver/pressure-based yes
  ;
  define/models/viscous/ke-standard yes ke-realizable yes
  define/models/viscous/near-wall-treatment enhanced-wall-treatment yes
  ;-----------CONSTANT DENSITY ---------
  define/materials/change-create air air y constant 1.187 n n y constant 0.0000182 n n n
  ;-----------IDEAL-GAS ----------------
  define/materials/change-create air air yes ideal-gas yes polynomial 
  3 1033.33 -0.196044 3.93365e-4 yes polynomial 3 6.24978e-6 9.73517e-5 -3.31177e-8 
  yes sutherland two-coefficient-method two-coefficient-method 1.458e-6 110.4 yes 28.966 no no no no no
  ;-----------As on older version-------
  define/boundary-conditions/zone-type inlet pressure-inlet
  define/boundary-conditions/pressure-inlet inlet no 0 no 0 no 300 no yes no yes 5 0.1
  define/boundary-conditions/zone-type outlet pressure-outlet
  define/boundary-conditions/pressure-outlet outlet no 0 no 0 no 300 no yes no yes 5 0.1 
  ;-----------As on version 19.X--------
  define b-c zone-type z-right mass-flow-outlet
  define b-c zone-type z-right mass-flow-inlet 
  define b-c zone-type z-right pressure-outlet 
  define b-c zone-type z-right mass-flow-inlet 
  define b-c set vel-inlet z-right z-left () vmag no 1.25
  define b-c set vel-inlet z-right () vel-spec turb-intensity 2 () turb-visc-ratio 5 ()
  def b-c set m-f-i z-right () dir-spec no yes 
  def b-c set m-f-i z-right () mass-flow no 1.50 ()
  def b-c set m-f-i z-right () t-i 5 ()
  def b-c set m-f-i z-right () t-v-r 10 ()    
  ;
  define/operating-conditions operating-pressure 101325
  define/operating-conditions reference-pressure-location 0 0 0
  define/operating-conditions gravity no
  ;
  ;Define Discretization Scheme
  ;0-1st UDS, 1->2nd UDS, 2->Power Law, 4-> QUICK, 6->3rd Order MUSCL
  solve/set/discretization-scheme density 1
  solve/set/discretization-scheme mom 1
  solve/set/discretization-scheme k 1
  solve/set/discretization-scheme epsilon 1
  solve/set/discretization-scheme temperature 1
  ;
  ;Press: 10->Std, 11->Linear, 12-> 2nd Order, 13->Body Force Weighted, 14-> PRESTO!
  solve/set/discretization-scheme pressure 12
  ;
  ;Flow: 20->SIMPLE, 21->SIMPLEC, 22->PISO
  solve/set/p-v-coupling 21
  ;
  ;Define Under-Relaxation Factors: method varies based on PV-coupling
  ;SIMPLE/SIMPLEC
  solve/set/under-relaxation body-force 0.8
  solve/set/under-relaxation k 0.8
  solve/set/under-relaxation epsilon 0.8
  solve/set/under-relaxation density 0.8
  solve/set/under-relaxation mom 0.4
  ;
  ;COUPLED with Psuedo-Transient
  solve/set/psuedo-under-relaxation mom 0.4
  ;
  solve/set/under-relaxation pressure rf
  solve/set/under-relaxation turb-viscosity 0.8
  solve/set/under-relaxation temperature 1.0
  solve/set/limits 50000 150000 250 400 1e-14 1e-20 40000
  ;
  solve/monitors/residual convergence-criteria 1.0e-6 1.0e-6 1.0e-6 1.0e-6 1.0e-6 1.0e-6
  solve/monitors/residual plot y
  solve/monitors/residual print y
  ;
  ; Initialize the solution and set auto-save data frequency: 3 options
  /solve/initialize/hybrid-initialization
  ;
  /solve/initialize/compute-defaults all-zones
  ;
  /solve/initialize/set-default/k 0.01
  /solve/initialize/set-default/e 0.01
  /solve/initialize/set-default/pressure 10
  /solve/initialize/set-default/temperature 300
  /solve/initialize/set-default/x-velocity 0.1
  /solve/initialize/set-default/y-velocity 0.1
  /solve/initialize/set-default/z-velocity 0.1
  ;
  /file/auto-save/data-frequency 200
  /file/auto-save/case-frequency if-case-is-modified
  /file/auto-save/retain-most-recent-files yes
  ;Field Functions
  /define/custom-field-functions/define "vort1" dz_velocity_dy-dy_velocity_dz
  /mesh/modify-zones/slit-interior-between-different-solids
  ;-----------Steady State Runs---------
  /solve/iterate 2000
  ;-----------Transient Runs------------
  solve/set/data-sampling y 1 y y
  solve/set/time-step 0.00001
  solve/set/adaptive-time-stepping y n 0.01 1.50 0.000001 0.001 0.5 2 5
  solve/dual-time-iterate 10000 20
  ;-----------Post-Processing-----------
  surface/line-surface L1 0.0 1.0 5.0 1.0
  surface/point-surface P1 5.0 0.5
  surface/plane-surf-aligned newsurf refsurf 0.0 0.25 0.0
  solve/monitors/surface/set-monitor P1 "Area-Weighted Average" pressure P1 () n n y P1.txt 1 y flow-time
  ;
  ;Save pressure xy plots of lines
  plot/plot y PL1 n n n pressure y 1 0 L1 ()
  plot/file PL1
  display/save-picture PL1.png
  plot/plot y PL1 n n n x-velocity y 1 0 L1 ()
  plot/file XVL1
  display/save-picture XVL1.png
  ;
  parallel/timer/usage
  report/system/proc-stats
  report/system/sys-stats
  report/system/time-stats
  ;
  file/confirm-overwrite yes    
  exit yes
Scheme command to turn on exit on error is: (set! *cx-exit-on-error* #t). To write the data file only, execute the following Scheme command before iterating: (rpsetvar 'checkpoint/write-case? #f)

The list of all the SCHEME codes impemented in FLUENT is summarized in attached file. It is being categorized into appropriate steps of simulation activites.


SCHEME Summary: Not all the built-in functions available in standard SCHEME are incorporated into FLUENT. For example, string-trim, string-prefix, string-suffix, string-replace... do not work in FLUENT TUI.

  • Statements are always included in small brackets such as (...)
  • Semi-colon ; is used at the beginning of a line to comment it, Comma , is used to accept default value in a command, () are used to define a list of selection. For instance (d1 d2 d3) or d1 d2 d3 () would both choose the three named zones and end the list.
  • Tilde (~) immediately followed by a newline ignores the newline and any following non-newline whitespace characters. With an @, the newline is left in place, but any following whitespace is ignored. This directive is typically used when control-string is too long to fit nicely into one line of the program
  • Boolean: #t = true, #f = false. Along with format statement, #f is used to return the output as a string. #t: destination port is the current-output-port. Refer to "Common Lisp" documentation for additional information.
  • #f: this may also get printed while using loops such as a 'do' loop. This is the return value if the loop is not provided a return expression. In other words, if no return value/expression is provided, 'do' loop will return either '#f' (meaning false) or '()' (meaning nothing).
  • Port: Ports represent input and output devices. To Scheme, an input port is a Scheme object that can deliver characters upon command, while an output port is a Scheme object that can accept characters.
  • "string" is a string, 'string is a symbol. No distinction between variable types (Integer, Real, String, ...). Like most of the programming languages: string is written as a sequence of characters enclosed within double quotes " ". To include a double quote inside a string, precede the double quote with a backslash \ (escape it).
  • Example of strings: (define fn "backStep") (ti-menu-load-string (string-append "file read-case-data " fn ".cas")). Note the space after 'read-case-data'.
  • (symbol-bound? 'symbol (the-environment) ) - check if a symbol is defined (bound)
  • (symbol-assigned 'symbol (the-environment)) - check if a symbol is assigned a value
  • (define x 3) - x = 3
  • LISP and hence SCHEME uses prefix notation where operators are written before their operands. Thus: a * ( b + c ) / d is expressed as (/ (* a (+ b c) ) d)
  • LISP programs have 3 basic building blocks − atom, list and string
  • (+ 2 4 5) = 11, (/ 6 3) = 2, (/ 2) = (/ 1 2) = 0.5
  • Function f(x) is called as (f x) such as (abs x), (sqrt x), (expt xy) = xy, (exp x) = ex, (log x) = ln(x), (sin x), (cos x), (atan x), (atan y x) = arctan(x/y)...
  • (remainder 45 6) = 3, (modulo 5 2) = 1, (truncate x), (round x), (ceiling x), (floor x), (max x y ...), (min x y ...) e.g. from a list search for maximum: (apply max (1 5 8 3 4)) = 8
  • (define y '(+ x 2)) = y is a 'list' with elements +, x, 2 and hence it is not evaluated. Tick mark ' is called quote and is a short-hand for (quote ...) call. It does not create a list, it is used to return something without evaluation.
  • (eval y (the-environment)) = 5, 'list' y interpreted as a SCHEME command
  • Use quote when you pass some static data (variable or list). For example, '(z) will be passed to cx-gui-do as is, variable 'z' will not be substituted and will stay as a symbol z Equality of numbers: (= a b), equality of objects: (eq? a b) or (equal? a b), same value objects: (eqv? a b)
  • Relations: (positive? x), (negative? x) (< a b) (> a b) (<= a b) (>= a b)
  • Boolean functions: (not a), (and a b c ...), (or a b c ...)
  • List: By definition, all lists have finite length and are terminated by the empty list. (Define zNames '(w-bot w-top vi-front po-rear symmetry)). (list object ...) - returns a list of its arguments. e.g. (list 'a (+ 3 4) 'c) = (a 7 c)
    • First item of a list: (car zNames) = w-bot
    • Rest of a list (i.e. list without first element): (cdr zNames) = (w-top vi-front po-rear symmetry)
    • Number of list elements: (length zNames) = 5
    • (list-ref xlst i): get ith item from list named 'xlst', similarly get head and tail items of a list: (list-head xlst n) / (list-tail xlst n)
    • Nested (car cdr) is 'cadr': (cadr x) = (car (cdr x)). (cadr '(a 5 b 8) ) = 5
    • (list-union list-1 list-2 list-3), (list-intersection list-1 list-2 list-3), (list-subtract list-1 list-2)
    • cons pushes item into a list that already exists
    • null? object: returns #t if object is the empty list otherwise returns #f
    • (string->list "xyz-123") = (x y z - 1 2 3) - note the output is within parentheses as it is a list. (list->string ((string->list "xyz-123")) = xyz-123
  • Similar to the %-character in C the tilde (~) controls a pattern.
  • Format commands:
    • ~a: placeholder for a variable in general format (string without "")
    • ~d: integer number
    • ~04d: integer with zeros on the front is always 4 digits fill ( 5 is about 0005). e.g. this is important for file names.
    • ~f: floating-point number
    • ~4.2f: floating point number, a total of 4 characters long, 2 digits after the decimal: 1.2 will be 1.20
    • ~s: string with "" included: from (format #f "string: ~s!" "text") = "text"!
  • \n: newline character line feed, \" = " i.e. the double quotes are escaped by backslash.
  • (display expression) - write a printable representation of 'expression' to the default output port. (newline) - writes a newline character to the default output port.
  • (format #f "~6.4f" avgPr) - format AvgPr with 4 digits after decimal place
  • Vector or Array operations
    • (vector expr1 expr2 . . .) - creates a new vector containing the values of the given expressions. Vector elements are 0-indexed.
    • (make-vector n [expression]) - creates a new vector of 'n' elements each initialized to the value of the given 'expression' when provided. [...] indicates this is optional.
    • (vector-ref v n) - returns the element at position 'n' of vector v, where 0 is the index of the first element of the vector. Error will be reported if n < 0 or n is > the last element in the vector.
    • (vector-set! v n expression) - sets the value at position 'n' of vector v to the value of the 'expression'.
  • (zone-id->name zid) returns (displays in TUI console) the name of zone having id 'zid' Equivalent commands in FLUENT Pre-Post are (thread-name->id "solid01") and (thread-id->name 123). (get-thread-by-name) is not defined but (%get-thread-by-name) works.
  • Define a variable to store ID of a zone: (rp-var-define 'iz 1 'integer #f). '/' is allowed character in variable names which is meant to categorise the variables as per the need.
  • Set the value of zone ID to the variable: (rpsetvar 'iz (zone-name-> 'front))
  • Use the value of zone ID: (rpgetvar 'iz)
  • Wildcard character * on its own will only chose all entities, (*) will chose all entities and close the list
  • Obtain a list of all face zones: (define all-face-zones (get-face-zones-of-filter '*)), (get-face-zones-of-filter '*): get list of all zone names (note wildcard character *), Works in FLUENT Mesher (Tgrid) only). Refer to Query and Utility Functions section of User's Guide.
  • Obtain a list of all cell zones: (define all-cell-zones (get-cell-zones-of-filter '*)), (get-cell-zones-of-filter '*): get list of all 'cell' zone names (note wildcard character *), Works in FLUENT Mesher (Tgrid) only).
  • (inquire-thread-names) in Pre-Post prints names of all the zones including of type 'Interior' and it does not accept wildcard characters.
  • Get number of facets of a face zone: (tg-get-thread-count zID) where zID is the zone ID
  • RP in (rpgetvar) refers to refers to user-specifiable model macros. Similarly, CX in (cxgetvar) refers to environmental Fluent-related variable (Cortex)
  • Evaluate a list as a Scheme command in the TUI: (define y '(1 2 3)) (eval y (the-environment))
  • (system "command"): Run command in the system shell
  • (gui-show-partition) prints statistics of grid partitions, (gui-memory-usage) gives information related to memory used by the solver
  • Most (not all) Schemes have built-in support for regular expression (regex or regexp) matching using the same regular expression syntax found in languages such as Perl and Javascript.
  • Conditionals in Scheme: cond works by searching through its arguments in order. It the first arguemnt returns #t then returns the second element of the this argument. It the first arguemnt returns #f then goes on to evaluate second argument and if it returns #t then returns the second element of the second argument. It the second argument also returns #f the it returns the third and last element. (cond [(equal? 'one 'won) '1] [(equal? 'two 'too) '2] [else 'spelling-error]): this returns "spelling-error" as the first two arguments will return #f.
  • Predicates are functions (like + or *) which return Boolean values (#t or #f). Predicates are usually given a '? as the last character of their name as a mnemonic device.
  • Binding constructs: let, let* and letrec give Scheme a block structure where the syntax of the three constructs is identical, but they differ in the regions they establish for their variable bindings. In a let expression, the initial values are computed before any of the variables become bound. In the let* expression, the bindings and evaluations are performed sequentially and in letrec expression, all the bindings are in effect while their initial values are being computed, thus allowing mutually recursive definitions.

(if(not(rp-var-object 'hflx-id))
  (rp-var-define 'hflx-id 10 'integer #f) ()
)
(rpgetvar 'hflx-id) -> This will print 10 in console.
(if (zone-name->id 'wall_hflx)
  (rpsetvar 'hflx-id (zone-name->id 'wall_hflx))
  (rpsetvar 'hflx-id 10)
)

TUI commands that take single or multiple zone names support the use of wildcards. For example, to copy boundary conditions (copy-bc) to all zones of a certain type, use a * in the name of the zone to which you want to copy the conditions. Example: report surface-integrals facet-avg w-htc* , temperature no

Similarly, following script can be used to change all walls having names ending in 'shadow' to type coupled: define b-c wall *shadow () 0 n 0 y steel y coupled n n 1

(list-bc "settings.bc") prints a list of type (zone name : zone type) where the input file "settings.bc" were created by TUI operation "file write-settings settings.bc".

Set Wall Rotation for zone having id ZID about X-axis passing through [XC YC ZC] and speed RPM: /define/b-c/wall ZID y n n n y n n 0 n 0 n RPM XC YC ZC 1 0 0

ZID Zone ID or name of the zone
y Change current value?
n Change shear-bc-noslip?
n Change rough-bc-standard?
n Wall motion relative to cell zone?
y Apply rotation velocity?
n Define wall velocity components?
n Use profile for wall-roughness height?
0 Wall roughness height
n
0
n
RPM Wall rotation speed in RPM
XC X-coordinate of a point on axis of rotation
YC Y-coordinate of a point on axis of rotation
ZC Z-coordinate of a point on axis of rotation
1 Direction cosine of X-axis
0 Direction cosine of Y-axis
0 Direction cosine of Z-axis

Set volumetric heat source for a zone with id ZID and material MATNAME: /define/b-c/solid ZID y MATNAME y 1 y 1250 n no n 0 n 0 n 0 n 0 n 0 n 0 n no n

ZID Zone ID or name of the zone
y Change current value?
MATNAME Name of the material defined
y Specify source terms?
1 Number of energy sources
y Use constant or expression for Energy 1
1250 Heat density in [W/m3]
n Specify fixed value?
no Frame motion?
n Use profile for reference frame X-origin of rotation axis?
0
n Use profile for reference frame Y-origin of rotation axis?
0
n Use profile for reference frame Z-origin of rotation axis?
0
n Use profile for reference frame X-component of rotation axis?
0
n Use profile for reference frame Y-component of rotation axis?
0
n Use profile for reference frame Z-component of rotation axis?
0
n Mesh motion?
no Solid motion (enter 'no' and not 'n')
n Solid motion (enter 'no' and not 'n')

FLUENT Scheme Error Debugging

(display get-thread-list): output is #[compound-procedure]

(display (get-thread-list)): it results in error with following message:

  Error: eval: unbound variable

  Error Object: name --- this indicates the argument is missing for get-thread-list

Similarly, (display (get-thread-list '*shadow)) shall print all zones with names ending in shadow. (display (get-thread-list 'solid*)) will print all the zones whose names start with 'solid'. When the error message is only Error: eval: unbound variable, it implies that the code is not defined in FLUENT Scheme.

Scheme codes which try to access mesh elements shall make the program crash. For example, (get-all-thread) or (display get-all-thread) shall make FLUENT session crash. However, (map thread-id (get-all-threads)) shall print the ID of all threads (zones) in the set-up (case) file. Similarly (get-threads-of-type 'interior) or (get-threads-of-type 'velocity-inlet) make the cortex crash, (map thread-id (get-threads-of-type 'wall)) prints the IDs of all zone of type wall

As explained in later sections: "Think of a ‘zone’ as being the same as a ‘thread’ data structure when programming UDFs. Thus: node thread = grouping of nodes, face thread = grouping of faces, cell thread = grouping of cells. A domain is a data structure in ANSYS FLUENT that is used to store information about a collection of node, face threads, and cell threads in a mesh." There would be only 1 domain in single phase flow simulations including conjugate heat transfer with only 1 flow medium.

In FLUENT, a 'surface' is defined as any plane created for post-processing purposes and not the one used in computation. Hence, Scheme codes working on surface shall not accept boundary face zone as input. e.g. (define tp (surface-area-average (list (surface-name->id "plane-10")) "temperature")) works but (define tp (surface-area-average (list (surface-name->id "w-htc-x")) "temperature")) does not work where w-htc-x is a face zone with specified HTC boundary conditions. (list (surface-name->id) "plane-10") shall print (10) as output. However (surface-area-average) will give following error:
  Error: eval: unbound variable
  Error object: s


Access each member of a list
The functions 'car' and 'cdr' can be used in combination to explore a list.
(define (print-list items)
  (for-each 
    (lambda (ii)
      (display ii)  (display " ") (newline)
    )
    items
  )
  (newline)
) (print-list '(a b c))

This function prints each member of the list on separate lines. The following code creates 'sum' function to add each member of the list. Note 'list' is a reserved word in SCHEME to define built-in variable. Hence, do not use the word 'list' as an argument to a function.

(define (sum items)
  (if (null? items) 0
    (+  (car items)  (sum (cdr items)  )
    )
  )
)
(sum '(5 10 15)) = 30. Now and 'avg' function can be defined to find 'average' of the numbers in a list.
(define (avg ist)
  (/ (sum ist) (length ist) )
)
(avg '(5.0 10.0 15.0) ): gives output 10.0.

Thus following function can be used in FLUENT mesher to rename solid (cell) or/and boundary (face) zones or add a prefix / suffix to face and/or cell zones. The code to rename only cell zones are defined below. Note that strings (such as zone names) with hyphen '-' needs to be converted into string using format ~s option.

(define (rename-cell-zones items)
  (for-each 
    (lambda (zid)
      (define zold (zone-id->name zid) )
      (define zolx (format #f "~s" zold) )
      (define znew (string-append zolx "_mat") )
      (ti-menu-load-string (string-append "mesh manage name " zolx " " znew) )
    )
    items
  )
  (newline)
) (rename-cell-zones (get-cell-zones-of-filter '*))

Split String: Splits a string into a list of strings separated by the delimiter character such as comma, space, colon... Few important procedures related to string manipulations are: string-ref string idx - (which returns character string[idx], using 0-origin indexing), substring string start end - returns a string containing the characters of string beginning with index 'start' (inclusive) and ending with index 'end' (exclusive). string-take str nc - returns a string containing the first 'nc' charactoers of string 'str', string-drop str nc - returns a string containing all but the first 'nc' character of string 'str', string-take-right str nc - returns a string containing the last 'nc' characters of string 'str', string-drop-right str nc - returns a string containing all but the last 'nc' characters of string 'str'. Out of these functions, only string-ref and substring works in FLUENT Mesher.

(define (str-split str ch)
  (let 
    (
      (len (string-length str))
    )
    (letrec
       (
         (split 
           (lambda (a b)
             (cond
               (
                 (>= b len) (if (= a b) '() (cons (substring str a b) '()))
               )
               (
                 (char=? ch (string-ref str b)) (if (= a b)
                 (split (+ 1 a) (+ 1 b))
                   (
                     cons (substring str a b) (split b b))
                   )
               )
               (else (split a (+ 1 b)))
             )
           )
         )
       )
       (split 0 0)
    )
  )
) 
(str-split "abc:def:pqr" #\:) - output = (abc def pqr). (str-split (format #f "~s" "abc:def:pqr") #\:) - output = ("abc def pqr"). Similarly, (list-ref (str-split "abc:def:pqr" #\:) 1) = def.

Join list of strings with delimiter

(define (string-join lst delimiter)
  (if (null? lst) ""
    (let loop ((result (car lst)) (lst (cdr lst)))
       (if (null? lst) result
          (loop (string-append result delimiter (car lst))
             (cdr lst)
          )
       )
    )
  )
) 
(string-join '("abc" "123" "xyz") "-") = abc-123-xyz

IF-Loop

(if cond true-value false-value) - 'cond' is a boolean expression that is either #t (true) or #f (false). ((if #f + *) 3 4) = (* 3 4) = 12, ((if #t + *) 2 5) = (+ 2 5) = 7. (if (> 1 0) 'yes 'no) = yes, if (> 2 3) 'yes 'no) = no
(if (cond 
 (begin  
   (if ... True-value ) 
 )
 (begin 
   (else ... False-value)
 )   
)

Conditionals - similar to IF-Loop

(cond
  (test1 value1) 
  (test2 value2) 
  ... 
  (else value)
)
(define x 5)
(cond 
  ((> x 3) 'pass)
  ((< x 3) 'fail)
  (else 'retry)
)  
  
e.g. Check if a boundary zone, plane... exists or not
(if 
 (equal? (surface-name-> id 'planeXY)  
  #f
 )
)
(surface-name/id? 'planeXY) produces #t is a surface named 'front' exists. Similarly, (display (zone-name-> id 'water)) shall display/print the ID of zone named 'water'. 
Define a boundary condition if a zone-name exists. The syntax uses 'member' as in (member x LIST) which return the first item or sub-list of 'LIST' whose 'car' (the first element) is 'x' or returns '#f' if 'x' does not occur in the list. Equal? can be used for comparison. The script also uses 'map' which is a higher order procedure: (map fn list-1 list-2 . . .): Apply 'fn' to each element of all the input lists and collect the return values into a list which is returned from 'map'.
(if 
 (member 'bc-inlet 
  (map thread-name 
   (get-face-thread)
  )
 )
 (begin
  (ti-menu-load-string "define b-c vel-in n n y y n 5.0 n 0 n n y 5 10")
 )
)
Wildcard character '*' can be used to specify zone names. E.g. (fluid*) refers to all the zones starting with 'fluid'. Since this method of refering multiple zones creates a list, it has to be included in (...) i.e. (fluid*) and not fluid*. e.g. "report volume volume-average (fluid*) temperature no". (inquire-cell-threads) and (inquire-grid-threads) print the thread or zone ID and zone type as pair such as (121 . 1). The zone type defined in ANSYS FLUENT are: 1 - Solid, 2 - Interior, 3 - Wall, 4 - Inlet (pressure-inlet, inlet-vent...), 5 - Outlets (pressure-outlet, exhaust-fan...), 10 - velocity-inlet, 20 - mass-flow-inlet or mass-flow-outlet, 24 - Interface, 37 - Axis.

DO-Loop

(do 
 (
   (x start-x (+ x delta-x))  ((> x x-end))
   ... loop body ...
)
Merge free and non-free odes with increasing value of tolerance:
(do 
 ( (i 10 (+ i 10)) (> i 50) )
  (ti-menu-load-string (format #f "boundary/merge-nodes (*) (*) no yes ~a" i) )
 )
)

Create multiple planes every 0.2 [m]: do(x = 0, x = x + 0.2,  x < 3.0)
(do 
 ( (x 0 (+ x 0.2)) (>= x 3.0) )
  (ti-menu-load-string (format #f "surface iso-surface x-coordinate x-3.1f ~a () 3.1f ~a ()" x x)) 
)
Output: Creates the following text interface commands: 
surface iso-surface x-coordinate x-0.0 () 0.0 () 
surface iso-surface x-coordinate x-0.2 () 0.2 () 
surface iso-surface x-coordinate x-0.4 () 0.4 () 
... 
surface iso-surface x-coordinate x-3.0 () 3.0 ()

To add a '+' symbol for positive numbers:
(if (> x = 0)
  "+" "") x x)

Read multiple data files (usually created during transient runs) and save images of a pre-defined contour plot in PNG format

(define datfile "Run-1-A-")
(define suffix ".000.dat.gz")
(define m 10)
(define n 50)
(define s 5
(do 
 (
  (i  m (+ i  s) )
 )
 (
  (> i  n)
 )
 (ti-menu-load-string (string-append "file read-data " datfile (number->string i) suffix))
 (ti-menu-load-string "display objects display contour-vel")
 (define pic (string-append datfile (number->string i) ".png"))
 (ti-menu-load-string (string-append "display save-picture " pic))
) 

Local Function: lambda - a lambda expression evaluates to a procedure. The result of the last expression in the body will be returned as the result of the procedure call.

e.g.(lambda (x) (+ x x)): the function or procedure || ((lambda (x) (* x x)) 5) = 25 - the value is returned by procedure

(lambda (arg1 arg2 ...) 
  ... 
  function value
)

FOR EACH-Loop

Set temperature and wall velocity for several BC wall zones:
(for-each 
 (lambda (zone) 
  (ti-menu-load-string 
   (format #f "def b-c wall ~a 0 y steel y temperature n 300 n n n n 0 no 0.5 no 1" zone) 
  ) 
 (newline) (display "") 
 )
)

Create a function:

(map 
 (lambda(x)
   (+ (* x x) 5.0)
 )
 '(1 2 3)
) 
Output: (6, 9, 14)

CASE-Loop: discrete values of a variable - If x in one of the lists found (eg in (x11 x12 x13 ...)), then the corresponding value is returned (value1).

(case x 
 ((x11 x12 x13 ...) 
    value1
 ) 
 ((x21 x22 x23 ...) 
    value2
 ) 
 ... 
 (else value)
) 

Boundary condition for specified heat flux: def b-c wall top 0 n 0 y steel n n 2000 n n n n 0 no 0.5 no 1. The default setting in FLUENT is aluminum as material, heat flux as boundary conditions and no-slip stationary walls.


Monitor Points

Define velocity inlet b.c. by components: def b-c v-i bc_inlet n y y n 0 y n 1.0 n 2.0 n 3.0 n n y 5 10
Define velocity inlet b.c. by magnitude and direction: def b-c v-i bc_inlet y y n 5.0 n 0 y n 0.707 n 0 n 0.707 n n y 5 10
solve report-definitions add mf-inlet flux-mass-massFlow zone-names mf-inlet ()
solve report-files add mf-inlet report-definitions mf-inlet () file-name mf-inlet.out print yes ()
solve report-definitions add p-inlet surface-areaavg field pressure surface-names srf-1 srf-2 ()
Field (flow) variables in FLUENT: pressure, entropy, x-surface-area, pressure-coefficient, total-energy, y-surface-area, dynamic-pressure, internal-energy, z-surface-area, rel-total-temperature, x-coordinate, dp-dx, wall-temp-out-surf, y-coordinate, dp-dy, wall-temp-in-surf, z-coordinate, dz-dp...

Define zone name as variable and use it in post-processing:

(define zName '(vi_inlet))
(display zName)
(define avgPr 
  (pick-a-real
    (format #f "/report/s-i/a-w-a ~a pressure no ()" zName)
  )
)
(display avgPr) 
Note: (display (format "~6.4f" avgPr)) will produce 0.0247*the-non-printing-object*. The statement (display (format #f "~6.4f" avgPr)) will give the desired output 0.0247.

Display a message if certain criteria is met: e.g. if temperature is less than or equal to 373 [K], report 'pass' or 'fail'.

(if 
 (<= 373
  (pick-a-real 
   (format #f "report/surf-integral/a-w-a w-cht-hx temperature no)
  )
 )
 (display "pass") (display "fail")
) 

Export fluent zone names: this is applicable to FLUENT pre-post and not FLUENT Mesher. Once this journal is copy-pasted in TUI or read through a journal file, one need to type commmand (export-bc-names) in the TUI - including the parentheses.

(define (export-bc-names) 
  (for-each 
    (lambda (name) 
      (display 
        (format #f " {~a, \"~a\", \"~a\"}, \n" 
          (zone-name->id name) name (zone-type (get-zone name)) 
        )
      )
    )
    (inquire-zone-names)  
  ) 
) (export-bc-names)
(inquire-zone-names)-- this provides list of zone names to the 'for-each' loop. Fluent output:
(export-bc-names) 
{26, "w-top", "wall"}, 
{2, "fluid", "fluid"}, 
{29, "w-bot", "wall"}, 
{15, "w-side", "wall"}, 
{17, "inlet", "vi-inlet"}, 
{25, "default-interior", "interior"}

Rename Shadow Walls

Scheme script to rename shadow wall pairs. This code was downloaded from the public domain and variable names have been shortened a bit and text indented.

;------------------------------------------------------------------------------
; Scheme function to identify which interior zones are "immersed" in a certain
; fluid zone. To use it, load the Scheme function through
; File>Read>Scheme ... or through  (load "immersed.scm") and then use the TUI 
; command (for example): (imme-info 'fluidX)
; It will print 1 or several interior zones that are completely immersed into 
; the fluid zone specified. One of them is for sure the Default-Interior type
; associated with that fluid zone named fluidX
;------------------------------------------------------------------------------
(define (imme-info fzn)
  (let 
    (
      (id-fz (thread-name->id fzn)
      )
       (int-list (map thread-id (get-threads-of-type 'interior))
       )
    )
    (for-each 
      (lambda (id)
        (let 
        (
          (zz (inquire-adjacent-threads id))
          (id1)(id2))
          (set! id1 (car zz))
          (set! id2 (cadr zz))
          (if (eqv? id1 id2) 
            (if (eqv? id1 id-fz)
            (format "\n Interior zone "~a" is immersed in "~a" \n" (thread-id->name id) fzn)
            )
          )
        )
      ) int-list
    )
  )
) 

Change Boundary Condition at Flow Times

A Scheme code referenced from ANSYS Learning Forum is described below.

(cond
  ((and 
    (> (rpgetvar 'flow-time) 0.1) (< (rpgetvar 'flow-time) 0.2)
   )
     (ti-menu-load-string "define/b-c/z-t 6 wall")
     (ti-menu-load-string "define/b-c/z-t 7 pressure-outlet"))
  ((and 
    (> (rpgetvar 'flow-time) 0.5) (< (rpgetvar 'flow-time) 0.6)
   )
     (ti-menu-load-string "define/b-c/z-t 6 wall")
     (ti-menu-load-string "define/b-c/z-t 7 pressure-outlet"))

(else
  (ti-menu-load-string "define/b-c/z-t 7 wall")
  (ti-menu-load-string "define/b-c wall 7 no no no no 0 no 0.5")
  (ti-menu-load-string "define/b-c/z-t 6 pressure-inlet")
  (ti-menu-load-string "define/b-c pressure-inlet 6 yes no 0 no 0 no yes no no yes 2 5"))
)

Creating animation: Create animation from the data files of a transient simulation, single frames will be created for an animation. The names of the data files are numbered with initial, final value with a step size. Errors encountered during the execution of a Fluent command, or a termination by Ctrl-C will also cause the Scheme program to quit.

File names are twophase-0010.dat, twophase-0020.dat... and images generated are image-01.png, image-02.png... Note that 'hardcopy' has been replaced by 'picture' in version 2020-R1 though there is backward compatibiity.

(define datfile "twophase") 
(define f-index 10) 
(define l-index 100) 
(define delta 10) 
(define imgfile "image")
(define (time) (rpgetvar 'flow-time)) 
(define t0 0)
; ------------------------------------------------ ------------------------
;       Function to create frames for the film 
; ------------- ----------------------------------------------------------- 
(define (pp) 
 (let ((break #f)) 
  (ti-menu-load-string "display set hardcopy driver png")
  (ti-menu-load-string "display set hardcopy color-mode color")
  (do ((j f-index (j + delta)) (i 1 (+ i 1))) ((or (> j l-index) break))
   (set! break 
    (not
      (and
       (ti-menu-load-string (format #f "file r-d ~a ~04d.dat" datfile j))
       (begin (if (= i 1) (set! t0 (time))) #t)
       (ti-menu-load-string "display hardcopy ~a ~02d.png" imgfile i) 
      )
    )
   ) 
  ) 
  (if break 
   (begin (newline) (newline) 
    (display "Scheme interrupted!") 
    (newline)
   )
  )
 )
)

Simple example (disp)-function for contour-plot:
(define (disp) 
 (ti-menu-load-string "display contour temperature 300 500")
) 
Example (disp) function: overlay contours and velocity-vectors. To call the (disp) function for testing: (disp), call the function to generate the images: (pp).
(define (disp) 
 (and 
  (ti-menu-load-string (format #f "display lang set title \" Time 5.1fs = ~ \ "" (- (time) t0)))
  (ti-menu-load-string "display set overlays no") 
  (ti-menu-load - string "display temperature contour 300 500") 
  (ti-menu-load-string "display set yes overlays") 
  (ti-menu-load-string "display lang velocity vectors, velocity-magnitude 0.0 1.0 5 0") 
 ) 
)

GUI Components in FLUENT and SCHEME Script


Few examples form posts on cfd-online.com: This piece of code prints centroid of boundaries defined at type "velocity-inlet".

(display
 (map 
  (lambda (zone) 
   (format #f "~a: (~a,~a,~a)\n" zone 
    (pick-a-real
     (format #f "/report/surface-int/a-w-a ~a () x-coordinate no" zone)
    )
    (pick-a-real
     (format #f "/report/surface-int/a-w-a ~a () y-coordinate no" zone)
    )
    (pick-a-real
     (format #f "/report/surface-int/a-w-a ~a () z-coordinate no" zone)
    )
   )
  )
  (filter
   (lambda (zn) (eq? (zone-type (get-zone zn)) 'velocity-inlet)) (inquire-zone-names)
  )
 )
) 

Check whether a cell thread is adjacent to a face thread or not

(define (check_adjacency fluid_id face_id)
  (let 
    ( 
      (fluid_chk (inquire-adjacent-threads face_id)) (aa)
    )
    (set! aa (car fluid_chk))
    (if(eqv? aa fluid_id)
      (display "Face and Fluid adjacent.")
      (display "Face and Fluid not adjacent.")
    )
  )
) 

ANSYS FLUENT star-up customization: This can be complementary to options available under Preferences in latest versions (V2021...)

(let (old-rc client-read-case)
 (set! client-read-case
  (lambda args
    (apply old-rc args)
    (if (cx-gui?)
    (begin
      (rpsetvar 'residuals/plot? #t)
      ;Turning off convergence check
      (rpsetvar 'residuals/settings '(
        (continuity #t 0 #f 0.0001)
        (x-velocity #t 0 #f 0.0001)
        (y-velocity #t 0 #f 0.0001)
        (z-velocity #t 0 #f 0.0001)
        (energy #t 0 #f 1e-08)
        (k #t 0 #f 0.0001)
        (epsilon #t 0 #f 0.0001)
        )
      )
      (rpsetvar 'mom/relax 0.4)
      (rpsetvar 'pressure/relax 0.5)
      (rpsetvar 'realizable-epsilon? #t)
      (cxsetvar 'vector/style "arrow")
    )
    )
  )
 )
)

Read a custom color map or write an existing one. The procedure consists of: Loading the Scheme file >> (load "rw-colormap.scm") >> Reading a new color map: /file/read-colormap >> Writing an existing color map: /file/write-colormap. Reference: Fluent Tips & Tricks - UGM 2004 by Sutikno Wirogo and Samir Rid.

(define (write-cmap fn)
  (let (
    (port (open-output-file (cx-expand-filename fn)))
    (cmap (cxgetvar 'def-cmap))
    )
    (write (cons cmap (cx-get-cmap cmap)) port)
    (newline port)
    (close-output-port port)
  )
)
(define (read-cmap fn)
  (if (file-exists? fn)
    (let ((cmap (read (open-input-file (cx-expandfilename fn)))))
      (cx-add-cmap (car cmap) 
        (cons (length (cdr cmap)) 
         (cdr cmap)
        )
	  )
      (cxsetvar 'def-cmap (car cmap))
    )
    (cx-error-dialog
      (format #f "Macro file ~s not found." fn)
    )
  )
)
(define (ti-write-cmap)
  (let ((fn (read-filename "colormap filename" "cmap.scm")))
    (if (ok-to-overwrite? fn)
      (write-cmap fn)
    )
  )
)
(define (ti-read-cmap)
  (read-cmap (read-filename "colormap filename" "cmap.scm"))
)
(ti-menu-insert-item! file-menu
  (make-menu-item "read-colormap" #t ti-read-cmap "Read colormap from file")
)
(ti-menu-insert-item! file-menu
  (make-menu-item "write-colormap" #t ti-writecmap "Write colormap to file")
)  

Replace all occurrenece of characters in a string. Reference: stackoverflow.com/.../flexible-replace-substring-scheme. Note that this code require (prefix?) to work as it is not implemented in all Scheme environments.

(define (rplc-all input trgt src)    
  (let 
    (
      (input (string->list input))
      (trgt (string->list trgt))
      (src (string->list src))
      (trgt-len (string-length trgt))
    )
    (let loop ((input input) (acc '()))
      (cond ((null? input) (list->string (reverse acc)) )
          ((prefix? input trgt)
            (loop (list-tail input trgt-len)
              (reverse-append src acc)
            )
          )
           (else
             (loop (cdr input) (cons (car input) acc))
           )
      )
    )
  )
)
(rplc-all "w-htc_2" "-" "_) 

(let um (cx-add-menu "usrMenu" #\M)): it adds a menu named usrMenu in the top main menu bar with M underlined to indicate keyboard shortcut. The ID of the newly created menu is printed in console which can also be access by code (cx-get-menu-id "usrMenu"). To add items to this menau: (cx-add-item um "CFD Steps" #\O #f and (lambda () (system "chrome.exe https://cfdyna.com &")))

FLUENT SCHEME Command Error Message
In general the error message from Scheme commands in FLUENT is a bit cryptic, some gives an idea of missing arguments or inputs. Following sections describes the error messages and hints about missing arguments.

(scale-grid): This will give following errors:

(scale-grid) (scale-grid 0.01)
Error eval: unbound variable Error eval: unbound variable
Error Object: fx Error Object: fy
The code is expecting (unknown number of) arguments. The first one is denoted as fx The code is expecting (unknown number of) arguments. The second one is denoted as fy
As you can guess, scaling of mesh required three scaling factors. Hence, the correct synstax is (scale-grid 0.1 0.1 0.1)
Another example:
(color-list)
Error eval: invalid function
Error Object: ("foreground" "red" "blue" .... "salmon")
As you can guess, the output of code is a list which could not be processed. (display color-list) prints the list of colours ("foreground" "red" "blue" .... "salmon")
More examples:
(thread-domain-id) (thread-id), (domain-id)
Error eval: unbound variable Error eval: unbound variable
Error Object: thread Error Object: thread
As you can guess, the code is expecting a list of threads. However, (get-all-domains) makes the cortex crash but (map domain-id (get-all-domains)) shall print (1) for single-phase flow cases.

(inquire-grid) shall print summary of mesh such as (0 874 2056 342 2) where the numbers correspond to cells, faces and node. (map domain-type (get-all-domains)) prints (mixture). (map domain-type (get-all-domains)) prints (geom-domain). (fluent-exec-name) prints the path of executables (*.exe) files. (list-database-materials) prints the names of all materials defined inside ANSYS FLUENT. (get-database-material 'air) prints all the properties currently defined for material air. Note the single quote before the name for material.

More examples:
(thread-surface) (thread-surface 21)
Error eval: too few arguments(0) Error eval: too few arguments(1)
Error Object: #[primitive-procedure %zone-surface] Error Object: #[primitive-procedure %zone-surface]
The code is expecting (unknown number of) arguments. However, #[primitive-procedure %zone-surface] is a bit cryptic and difficult to guess.

(volume-integrals) results in error with message "Error eval: unbound variable". (%volume-integrals) also results in error with differnt message:
Error: eval: too few arguments(0)
Error Object: #[primitive procedure %volume-integrals]


Customization vs. Extensibility
Customization Extensibility
In-product operation Out of product feature expansion
Modify existng functionality, Create new feature Enhance a software package with minimum development

EXAMPLE OF UDF
Only velocities in Cartesian coordinates (Ux,Uy,Uz) are accessible through the UDF macros. Radial, tangential & axial velocities (Ur, Ut, Ua) within a fluid zone will need to be computed using the UDF itself. The UDF below can be used to define inlet velocity as a function of radius and time. It is assumed that the centre of inlet face is at origin.
  Note that in order to access UDF parameters in post-processing, UDM (User Defined Memory) needs to be initialized using GUI path: Parameters & Customization → User Defined Memory → Number of User-Defined Memory Location where the UDM numbering starts from 0. In your UDF, assign your variable to a specific UDM. E.g. F_UDMI(face, thread, 0) = U_txyz; C_UDMI(cell, threat, 0) = vol_heat_source; '0' here refers to the UDM number.

Note that the DEFINE_XX macros implement general solver functions that are independent of the model(s) being used in ANSYS Fluent. For example, DEFINE_ADJUST is a general-purpose macro that can be used to adjust or modify variables that are not passed as arguments. For example, modify flow variables (velocities, pressure...) and compute integrals of a scalar quantity over a domain which can be used to adjust a boundary condition based on the result. A function that is defined using DEFINE_ADJUST executes at every iteration and is called at the beginning of every iteration before transport equations are solved.

#include "udf.h"
DEFINE_PROFILE(U_txyz, thread, position) {
  /*position: Index of variable say 'U' to be set                 */
  real x[ND_ND];             /* Position vector of nodes          */
  real xi, yi, zi, r;
  face_t f;
  real R = 0.050;            /* Radius in [m]                     */
  real t = CURRENT_TIME;     /* Current time of simulation        */
  begin_f_loop(f, b)         /* Loops over all faces in thread 'b'*/
  {
    /* C_CENTROID(x,c,t): returns centroid in real x[ND_ND]       */

    F_CENTROID(x, f, b);    /* Gets centroid of face f            */
    
    /* x[ND_ND]: Position vector of nodes                         */
    xi = x[0]; yi = x[1]; zi = x[2];
    r = sqrt(xi*xi + yi*yi + zi*zi);
    F_PROFILE(f, b, position) = 2.0 + 0.5*sin(t/5)*sin(0.31416*r/R);
  } 
  end_f_loop(f, thread)
} 

Note: The constant ND_ND is defined as 2 for RP_2D (2D domain) and 3 for RP_3D (3D domain). It can be used when it is require to build a 2x2 matrix in 2D and a 3x3 matrix in 3D. Instead if ND_ND is used, the UDF will work for both 2D and 3D cases, without requiring any modifications.


Another example of UDF which can be used to define a linear translation and angular displacement to a cylinder of plate with dynamic mesh motion setting is described below.
/* Rigid body motion of a cylinder: translation and rotations,
can be used for a flapping plate if translation is set 0.    */

#include "udf.h"
/* -----  Define frequency of rotation / flapping in Hz.     */
  #define f 5.0  
/* -----  Define angular velocity in [rad/s].                */
  #define omega 2.0*M_PI*f
/* -----  Define maximum angular deflection in [rad]         */
  #define thetaMax M_PI/180
/* -----  Define linear translation in [m]                   */
  #define xMax 0.01;
  
DEFINE_CG_MOTION(TransRot, dt, cg_vel, cg_omega, time, dtime) {
  real angVel, linVel;
  
  linVel = xMax * omega * cos(omega*time);
  cg_vel[0] = linVel;
  cg_vel[1] = 0.0;
  cg_vel[2] = 0.0;
  
  /*cg_omega[0] -> wx, cg_omega[1] -> wy, cg_omega[2] - wz   */
  /*Axis of rotation is about origin and should be ensured.  */
  angVel = ThetaMax * omega * sin(omega*time);
  cg_omega[1] = angVel;
  cg_omega[2] = 0.0;
  cg_omega[3] = 0.0;
}

Summary of UDF commands
Exerpts from user manual: Think of a ‘zone’ as being the same as a ‘thread’ data structure when programming UDFs. Thus: node thread = grouping of nodes, face thread = grouping of faces, cell thread = grouping of cells. A domain is a data structure in ANSYS FLUENT that is used to store information about a collection of node, face threads, and cell threads in a mesh.
UDF thread domain hierarchy
  • Data Types: Node is a structure data type that stores data associated with a mesh point, face_t is an integer data type that identifies a particular face within a face thread, cell_t is an integer data type that identifies a particular cell within a cell thread, Thread is a structure data type that stores data that is common to the group of cells or faces that it represents.
  • NODE_X(node) = X-coordinate of node
  • NODE_Y(node) = Y-coordinate of node
  • NODE_Z(node) = Z-coordinate of node
  • F_NNODES(f, t) = number of nodes in a face
  • C_CENTROID(x, c, t) / F_CENTROID(x, f, t): = returns centroid in a 1x3 array real x[ND_ND]
  • F_AREA(a, f, t): returns face area (normal) vector in real a[ND_ND]
  • C_VOLUME(c, t) = volume of cell
  • C_NNODES(c, t) = number of nodes
  • C_NFACES(c, t) = number of faces
  • C_FACE(c, t, i) = global face index, corresponding to local face index i
  • C_R(c, t) / F_R(f, t) = Access cell / boundary face flow variable density
  • C_P(c, t) / F_P(f, t) = Access cell / boundary and interior face flow variable pressure
  • C_U(c, t) / F_U(f, t) = Access cell / boundary face flow variable x-velocity
  • C_V(c, t) / F_V(f, t) = Access cell / boundary face flow variable y-velocity
  • C_W(c, t) / F_W(f, t) = Access cell / boundary face flow variable z-velocity
  • C_T(c, t) / F_T(f, t) = Access cell / boundary face flow variable temperature
  • C_H(c, t) / F_H(f, t) = Access cell / boundary face flow variable enthalpy
  • C_K_L(c, t) = Access cell material property "thermal conductivity". 'L', 'T' and 'EFF' suffix is used for 'Laminar', 'Turbulent' and 'Effective' properties. For example, C_MU_L, C_MU_T and C_MU_EFF refers to 'Laminar', 'Turbulent' and 'Effective' viscosities respectively.
  • Similarly, K, NUT, D, O and YI can be added to C_ to access TKE, turbulent viscosity of Spalart-Allmaras model, TED (ε), specific dissipation rate (ω) and mass fraction respectively. Note that the UDF will result in fatal error if the TKE or TDR is accessed in a solid domain (thread).
  • F_FLUX(f, t) = Access face flow variable mass flux
  • d = Get_Domain(1) = Get domain using FLUENT utility. Here, domain_id = 1 is an integer for the mixture or fluid domain, but the values for the phase domains can be any integer greater than 1. E.g. porousDomain = Get_Domain(2);
  • Derivative macro: C_UDSI(c, t, VORTICITY_Z) = C_DVDX(c,t) - C_DUDY(c,t) = define z-component of vorticity
  • C_R_G(c, t), C_P_G(c, t), C_U_G(c, t) ... can be used to get gradient vector: {dp/dx dp/dy dp/dz)
  • The M1 suffix can be applied to some of the cell variable macros to access value of the variable at the previous time step (t - Δt). These data may be useful in unsteady simulations. For example, C_T_M1(cell, thread); returns the value of the cell temperature at the previous time step
  • Similarly, M2 suffix can be applied to some of the cell variable macros to access value of the variable at second previous time step (t -2Δt). These data may be useful in unsteady simulations. For example, C_T_M2(cell, thread); returns the value of the cell temperature at the previous to previous time step
  • PRINCIPAL_FACE_P(f,t) = test if the face is the principle face - not required for serial operation, applicable to compiled UDFs only
  • C_VOLUME = get the cell volume and accumulates it. The end result is total volume of each cell of respective mesh.
  • C_UDMI(c, t,0) = store result in user-defined memory, location index 0. The user-defined memory field gets saved to the data file and can be used to generate contours and any other post-processing activity.
  • The NV_ macros have the same purpose as ND macros, but they operate on vectors (that is, arrays of length ND_ND) instead of separate components.
    • NV_V: The utility NV_V performs an operation on two vectors. NV_V(a, =, x) will result in a[0] = x[0], a[1] = x[1] and a[2] = x[2]
    • Use of '+ =' instead of '=' in the above equation results in summation. NV_V(a, +=, x) will result in a[0] = a[0] + x[0], a[1] = a[1] + x[1] and a[2] = a[2] + x[2]
    • NV_VV performs operations on vector elements. The operation that is performed on the elements depends upon what symbol (-, /, *) is used as an argument. NV_VV(a, =, x, +, y) will yield a[0] = x[0] + y[0], a[1] = x[1] + y[1] and a[2] = x[2] + y[2]
    • NV_V_VS utility operates (+, -, *, /) a vector to another vector which is multiplied or divided by a scalar. NV_V_VS(a, =, x, +, y, *, 0.5) will result in 2D: a[0] = x[0] + y[0] * 0.5, a[1] = x[1] + y[1] * 0.5
    • NV_VS_VS utility operates (+, -, *, /) a vector to another vector where both are multiplied or divided by a scalar. NV_VS_VS(a, /, 2.0, x, +, y, *, 5.0) will result in a[0] = x[0] / 2.0 + y[0] * 5.0, a[1] = x[1] / 2.0 + y[1] * 5.0, a[3] = x[3] / 2.0 + y[3] * 5.0
  • Other NV_ operations:
    • NV_VEC(A) - declare vector A
    • NV_D(psi, =, F_U(f,t), F_V(f,t), F_W(f,t)) - define psi in terms of velocity field, NV_D(axis, =, 0.0, 1.0, 0.0), NV_D(origin, =, 0.0, 0.0, 5.0)
    • NV_VV(rvec, =, NODE_COORD(v), -, origin)
    • NV_S(q, =, 0.0), NV_S(psi, *=, F_R(f,t)) - multiplying density to get psi vector
    • NV_DOT(A, B) - dot product of the two vectors, NV_CROSS(A, B) - crosss product of the two vectors
  • boolean FLUID_THREAD_P(thread): Check if 'thread' is of type FLUID
  • Some macros are defined in 'mem.h' and not in 'udf.h'. Example includes: C_FACE_THREAD(c, t, i), C_FACE(c, t, i), C_R(c,t), C_P(c,t), C_U(c,t), C_V(c,t)... F_PROFILE.

DEFINE_ON_DEMAND is a general-purpose macro that can be used to specify a UDF that is executed as needed in ANSYS FLUENT, rather than having ANSYS FLUENT call it automatically during the calculation. UDF will be executed immediately, after it is activated, but it is not accessible while the solver is iterating. Note that the domain pointer d is not explicitly passed as an argument to DEFINE_ON_DEMAND. Therefore, if you want to use the domain variable in your on-demand function, you will need to first retrieve it using the Get_Domain utility.

Excerpt from UDF Manual: The following UDF, named on demand calc, computes and prints the minimum, maximum, and average temperatures for the current data field. It then computes a temperature function f(T) = [T − TMIN]/[TMAX − TMIN] and stores it in user-defined memory location 0. After the on-demand UDF is hooked, the field values for f(T) will be available in drop-down lists in postprocessing dialog boxes in ANSYS FLUENT. This field can be accessed by choosing User Memory 0 in the User-Defined Memory... category.

Note that this is for demontration purpose only as the features to find out maximum, minimum and volume-weighted average are avaialbe as standard post-processing operatons.
#include "udf.h"
DEFINE_ON_DEMAND(Tavg) {
/* declare domain pointer: it isn't passed as an argument to the DEFINE macro */
  Domain *d; 
  real tavg = 0.0;
  real tmax = 0.0;
  real tmin = 0.0;
  real tp, volm, vtot;
  Thread *t;
  cell_t c;
  /* Get the domain using ANSYS FLUENT utility */
  d = Get_Domain(1); 
  /* Loop over all cell threads in the domain */
  thread_loop_c(t,d) {
    /* Compute max, min, volume-averaged temperature */
    /* Loop over all cells */
     begin_c_loop(c,t) {
       volm = C_VOLUME(c,t); /* get cell volume */
       tp = C_T(c,t);   /* get cell temperature */
       if (tp < tmin || tmin == 0.0) tmin = tp;
       if (tp > tmax || tmax == 0.0) tmax = tp;
       vtot = vtot + volm;
       tavg = tavg + tp*volm;
    } end_c_loop(c,t)
    tavg /= vtot;
    printf("\n Tmin = %g Tmax = %g Tavg = %g\n",tmin,tmax,tavg);
    /* Compute temperature function and store in UDM*/
    /*(location index 0) */
    begin_c_loop(c,t) {
      tp = C_T(c,t);
      C_UDMI(c,t,0) = (tp-tmin)/(tmax-tmin);
    } end_c_loop(c,t)
  }
}

This UDF will print the volume of cells with temperature withing specified [in K] range.

DEFINE_ON_DEMAND(isoVolume) {
/* declare domain pointer: it isn't passed as an argument to the DEFINE macro */
  Domain *d; 
  real tmax = 300.0;   /* This value should in [K] */
  real tmin = 320.0;   /* This value should in [K] */
  real temp, volm, vtot;
  Thread *t;
  integer zid;
  cell_t c;
  /* Get the domain using ANSYS FLUENT utility */
  d = Get_Domain(1); 
  /* Loop over all cell threads in the domain */
  thread_loop_c(t, d) {
     vtot = 0.0;
    /* Loop over all cells */
     begin_c_loop(c,t) {
       tp = C_T(c,t); /* get cell temperature */
       if (tp <= tmax && tp >= tmax) {
         /*Get cell volume and add to total volume */
         volm = C_VOLUME(c,t); 
         vtot = vtot + volm;
       }
    } end_c_loop(c,t)
    zid = THREAD_ID(t);
    printf("\n Zone - %d -- Volume in specified range = %g \n", zid, vtot);
  }
}

UDF in Parallel Computing on Clusters

Serial solver contains Cortex and only a single ANSYS Fluent process.

The parallel solver contains 3 types of executable: Cortex, host, and compute node (or simply 'node' for short). When ANSYS Fluent runs in parallel, an instance of Cortex starts, followed by one host and n compute nodes, thereby giving a total of (n + 2) running processes. For this reason, UDF for parallel run will need to be developed such that the function will successfully execute as a host and a node process.

Example of operations that require parallelization of serial source code include the following:
  • Reading and Writing Files
  • Global Reductions, Global Logicals
  • Global Sums, Global Minimums and Maximums
  • Certain Loops over Cells and Faces
  • Displaying Messages on a Console, Printing to a Host or Node Process
List of parallel compiler directives:
/*--------------------------------------------------------------------*/
/* Compiler Directives                                                */
/*--------------------------------------------------------------------*/
#if RP_HOST       /* only host process is involved                    */
#if !RP_HOST      /*either serial or compute node process is involved */
  ...
#endif

#if RP_NODE       /* only compute nodes are involved                  */
#if !RP_NODE      /* either serial or host process is involved        */
  ...
#endif

#if PARALLEL     /* both host and compute nodes are involved, but not */
                 /* serial equivalent to #if RP_HOST || RP_NODE       */
#if !PARALLEL    /* only serial process is involved                   */
  ...
#endif

Depending upon a UDF, the UDF written in C language needs to be compiled before it can be used in FLUENT. Best a UDF should be compiled on a system with the same operating system (OS) and processor architecture as the compute cluster. Typically the compute nodes are diskless nodes with bare minimum boot image, it lacks a C or CPP programming environment (compiler, linker, libraries). Hence, it is not possible to compile a UDF in batch mode on a compute node of the Linux clusters.


More examples of FLUENT UDF
UDF for Temperature Dependent Viscosity
DEFINE_PROPERTY(visc_T, c, Tp)		{
  real mu; real a = C_T(c,t);  
  mu = 2.414e-05 * pow(10, 247.8/(Tp - 140));
  return mu;						
}

Compute area of a face zone:

 #include "udf.h" 
 real Ar1 = 0.0; 
 begin_f_loop(f, t) 
 if PRINCIPAL_FACE_P(f, t) {  
  /* compute area of each face */  
  F_AREA(area, f, t);   
  /*compute total face area by summing areas of each face*/  
  Ar1 = Ar1 + NV_MAG(area);   
 }  
 end_f_loop(f,t)  
 Ar1 = PRF_GRSUM1(Ar1);  
 Message("Area = %12.4e \n", Ar1); 

Compute volume of a cell zone:

 #include "udf.h" 
 real Vm1 = 0.0; 
 begin_C_loop(c, t) 
  /*compute total volume by summing volumes of each cell*/  
  Vm1 = Vm1 + C_VOLUME(c, t);   
 }  
 end_f_loop(c, t)  
 Vm1 = PRF_GRSUM1(Vm1);  
 Message("Volume = %12.4e \n", Vm1);

UDF: change time step value in Transient Simulation

This example, UDF needs to operate on a particular thread in a domain (instead of looping over all threads) and the DEFINE macro DEFINE_DELTAT used in UDF does not have the thread pointer passed to it from the solver. Hence, Lookup_Thread is required in the UDF to get the desired thread pointer.

 #include "udf.h"
 DEFINE_DELTAT(timeStep, d) { 
 real newTime = CURRENT_TIME; real oldT; real minT = 0.0; real maxT = 0.0;
 Thread *t; cell_t c; d = Get_Domain(1); 
 int zID = 1; Thread *t = Lookup_Thread(d, zID); 
 begin_f_loop(f, t) { /* Loop over all face elements*/
   oldT = F_T_M1(f, t); /* Get face temperature at previous time-step */
   if (oldT < minT || minT == 0.0) minT = oldT;
   if (oldT > maxT || maxT == 0.0) maxT = oldT;
 }
 end_f_loop(f, t)

 if(maxT < 100.0) 
  timeStep = 0.5; 
 else 
  timeStep = 0.1; 
 
 return timeStep; 
 } 

Density as function of temperature:

#include "udf.h"
DEFINE_PROPERTY(rho_T, c, Tp) {
  real rho;
  /* Get temperature of the cell in K and convert into C */
  real Tp = C_T(c,t) - 273.11; 
  real a0 =  999.8396;
  real a1 =  18.22494;
  real a2 = -7.92221e-03;
  real a3 = -5.54485e-05;
  real a4 =  1.49756e-07;
  real a5 = -3.93295e-10;
  real b =   1.81597e-02;

  rho = a0 + a1*Tp + a2*Tp*Tp + a3*pow(Tp, 3) + a4*pow(Tp, 4) + a5*pow(Tp, 5);
  rho = rho / (1 + b*Tp);
  return rho;						
}

Sample UDF for 6DOF case. DEFINE_SDOF_PROPERTIES (name, properties, dt, time, dtime) specifies custom properties of moving objects for the six degrees of freedom (SDOF) solver which includes mass, moment and products of inertia, external forces and external moments. real *properties - pointer to the array that stores the SDOF properties. The properties of an object which can consist of multiple zones can change in time, if desired. External load forces and moments can either be specified as global coordinates or body coordinates. In addition, you can specify custom transformation matrices using DEFINE_SDOF_PROPERTIES. The boolean properties[SDOF_LOAD_LOCAL] can be used to determine whether the forces and moments are expressed in terms of global coordinates (FALSE) or body coordinates (TRUE). The default value for properties[SDOF_LOAD_LOCAL] is FALSE.

#include "udf.h"
#include "math.h"
DEFINE_SDOF_PROPERTIES(valve_6dof, prop, dt, time, dtime) {
prop[SDOF_MASS] = 0.10; /*Mass of the valve in [kg] */
prop[SDOF_IZZ] = 1.5e-3;/*Mass moment of inertia about Z axis [kg/m^2]*/
/* Translational motion setting, use TRUE and FALSE as applicable */
prop[SDOF_ZERO_TRANS_X] = TRUE; /*Translation allowed in X-Direction? */
prop[SDOF_ZERO_TRANS_Y] = TRUE; /*Translation allowed in Y-Direction? */
prop[SDOF_ZERO_TRANS_Z] = TRUE; /*Translation allowed in Z-Direction? */
/* Rotational motion setting, use TRUE and FALSE as applicable*/
prop[SDOF_ZERO_ROT_X] = TRUE; /*Rotation allowed about X-Axis? */
prop[SDOF_ZERO_ROT_Y] = TRUE; /*Rotation allowed about Y-Axis? */
prop[SDOF_ZERO_ROT_Z] = FALSE; /*Rotation allowed about Z-Axis? */
/* Gravitational, External Forces/Moments: SDOF_LOAD_F_X, SDOF_LOAD_F_Y ... SDOF_LOAD_M_Z */
M = prop[SDOF_MASS]; Larm = 0.10 */
prop[SDOF_LOAD_M_Z] = -9.81 * M * Larm * sin(DT_THETA(dt)[2] ;
Message("\n 2D: updated 6DOF properties DT_THETA_Z: %e, Mz: %e, Mass: %e \n",
DT_THETA(dt)[2], prop[SDOF_LOAD_M_Z], prop[SDOF_MASS]);
}

Tips and Tricks on UDF / UFF
  • To write output to a file from UDF operation / loop: open a file using statement: FILE *fileName; fileName = fopen("udfOutput.txt", "a"); fprintf(fileName,"%g %g\n", x[0], source); fclose(fileName); However, all the fopen / fprintf / fclose commands are incompatible with parallel operation.
  • To send output to the console: Message("x = %g source = %g\n", x[0], source);)
  • In STAR-CCM+ du/dy = grad($Velocity[0]/grad($Centroid[1]), in FLUENT UDF: C_DUDY(cell, thread). Similarly, C_DVDX(cell, thread) can be defined.
  • Similarly in FLUENT, C_T_G(cell, thread)[0] returns the x-component of the cell temperature gradient vector.

Errors and Troubleshooting in FLUENT UDF
[Error message] line xx: structure reference not implemented ---There can be multiple reasons such as the UDF interpreter could not find required libraries (for example Visual Studio). Another reason can be that the C preprocessor is trying to interpret code that contains elements of C that the interpreter does not accommodate ((which is not supported).

If an UDF is interpreted which resulted in error, a fresh FLUENT session is needed to compile the UDF.


Accessing FLUENT from Python

pyAnsys: This is the module which can be used to access FLUENT commands from Python code.
ICEM CFD: Tck/Tk Examples
For loop to copy a point entity:
for {set i 1} {$i <= $NS} {incr i}  {  
  ic_geo_duplicate_set_fam_and_data point ps$j ps[expr {$j+2}] {} _0  
  ic_move_geometry point names ps[expr {$j+2}] translate "0 $L 0"  
  ic_geo_duplicate_set_fam_and_data point ps[expr {$j+1}] ps[expr {$j+3}] {} _0  
  ic_move_geometry point names ps[expr {$j+3}] translate "0 $L 0"  
  set j [expr {$i*10+1}]  
} 


Macros in STAR-CCM+
The first step in writing a JAVA macro for STAR CCM+ is to import the relevant packages. For example:
package macro;  - similar to #include "udf.h"
import java.util.*;  - similar to header files in C
import star.turbulence.*; - import turbulence model data
import star.common.*;   import star.material.*;
import star.base.neo.*; import star.vis.*;
import star.flow.*;     import star.energy.*;
import star.coupledflow.*;

// defineSim is the name of macro and the file name should be defineSim.java.
public class defineSim extends StarMacro {
  public void execute() {
    execute0();
  }
  
  //Get active simulation data
  Simulation getSim = getActiveSimulation();
  
  //Get domain named as FLUID and store it as 'cfd' - similar to Get_Domain in FLUENT UDF
  Region cfd = getSim.getRegionManager().getRegion("FLUID");
  
  //Set viscous model
  PhysicsContinuum pC0 = ((PhysicsContinuum) cfd.getContinuumManager().getContinuum("Physics 1"));
    pC0.enable(SteadyModel.class);
    pC0.enable(SingleComponentGasModel.class);
    pC0.enable(CoupledFlowModel.class);
    pC0.enable(IdealGasModel.class);
    pC0.enable(CoupledEnergyModel.class);
    pC0.enable(TurbulentModel.class);
    pC0.enable(RansTurbulenceModel.class);
    pC0.enable(KEpsilonTurbulence.class);
    pC0.enable(RkeTwoLayerTurbModel.class);
    pC0.enable(KeTwoLayerAllYplusWallTreatment.class);

  //Get boundary named INLET and velocity specification CLASS
  Boundary b1 = cfd.getBoundaryManager().getBoundary("INLET");
  VelocityProfile vP1 = b1.getValues().get(VelocityProfile.class);
  
    //Specify velocity normal to boundary with specified "MAGNITUDE and DIRECTION"
    //Note the word scalar in ConstantScalarProfileMethod.class
    b1.getConditions().get(InletVelocityOption.class).setSelected(InletVelocityOption.MAGNITUDE_DIRECTION);
    vP1.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(5.0);
	
    //Inlet velocity by its COMPONENTS, note 'vector' in ConstantVectorProfileMethod.class
    //b1.getConditions().get(InletVelocityOption.class).setSelected(InletVelocityOption.COMPONENTS);
    //vP1.getMethod(ConstantVectorProfileMethod.class).getQuantity().setComponents(5.0, 0.0, 0.0);
  
    //Set turbulence parameters - TURBULENT INTENSITY and VISCOSITY RATIO at INLET boundary
    TurbulenceIntensityProfile TI = b1.getValues().get(TurbulenceIntensityProfile.class);
    TI.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(0.02);

    TurbulentViscosityRatioProfile TVR = b1.getValues().get(TurbulentViscosityRatioProfile.class);
    TVR.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(5.0);
	
    //Specify fluid temperature in [K] at INLET
    StaticTemperatureProfile Tin = b1.getValues().get(StaticTemperatureProfile.class);
    Tin.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(323.0);
	
  //Get boundary named OUTLET and pressure boundary CLASS
  Boundary b2 = cfd.getBoundaryManager().getBoundary("OUTLET");
  StaticPressureProfile sP0 = b2.getValues().get(StaticPressureProfile.class);
    
    //Specify static pressure at OUTLET boundary
    b2.setBoundaryType(PressureBoundary.class);
    sP0.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(0.0);
  
    //Specify back flow turbulence parameters at OUTLET boundary
    TurbulenceIntensityProfile TI2 = b2.getValues().get(TurbulenceIntensityProfile.class);
    TI2.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(0.01);

    TurbulentViscosityRatioProfile TVR2 = b2.getValues().get(TurbulentViscosityRatioProfile.class);
    TVR2.getMethod(ConstantScalarProfileMethod.class).getQuantity().setValue(2.0);
	
    //Other options for reverse flow specifications
    b2.getConditions().get(BackflowDirectionOption.class).setSelected(BackflowDirectionOption.EXTRAPOLATED);
    b2.getConditions().get(BackflowDirectionOption.class).setSelected(BackflowDirectionOption.BOUNDARY_NORMAL);
    b2.getConditions().get(ReversedFlowPressureOption.class).setSelected(ReversedFlowPressureOption.ENVIRONMENTAL);
    b2.getConditions().get(ReversedFlowPressureOption.class).setSelected(ReversedFlowPressureOption.STATIC);
    b2.getConditions().get(ReferenceFrameOption.class).setSelected(ReferenceFrameOption.LOCAL_FRAME);
    b2.getConditions().get(ReferenceFrameOption.class).setSelected(ReferenceFrameOption.LAB_FRAME);
    b2.getConditions().get(KeTurbSpecOption.class).setSelected(KeTurbSpecOption.INTENSITY_LENGTH_SCALE);
    b2.getConditions().get(KeTurbSpecOption.class).setSelected(KeTurbSpecOption.INTENSITY_VISCOSITY_RATIO);
	
  //Save SIM file by specifying full path - note double backslashes
  getSim.saveState(resolvePath("C:\\STAR_CCM\\PipeFlow.sim"));
  
  //Close the simulation scene
  getSim.close(true);
}

Another macro recorded in STAR-CCM+ V14.x:
// STAR-CCM+ macro: Macro.java, Written by STAR-CCM+ 14.02.012
package macro; import java.util.*;
import star.common.*; import star.base.neo.*; import star.segregatedflow.*;
import star.material.*; import star.turbulence.*; import star.rsturb.*;
import star.vis.*; import star.flow.*; import star.kwturb.*;

public class Macro extends StarMacro {
 public void execute() { 
   execute0(); 
 }

 private void execute0() {
  Simulation sim_0 = getActiveSimulation();
  ImportManager IM_0 = sim_0.getImportManager();

  IM_0.importMeshFiles(new StringVector(new String[] {resolvePath("D:venturi.ccm")}), 
    NeoProperty.fromString("{\'FileOptions\': [{\'Sequence\': 42}]}"));

  FvRepresentation fvRep0 = ((FvRepresentation) 
    sim_0.getRepresentationManager().getObject("Volume Mesh"));

  Region region_0 = sim_0.getRegionManager().getRegion("fluid");
  fvRep0.generateCompactMeshReport(new NeoObjectVector(new Object[] {region_0}));

  sim_0.getSceneManager().createGeometryScene("Geometry Scene", "Outline", "Geometry", 1);
  Scene scene_0 = sim_0.getSceneManager().getScene("Geometry Scene 1");
  scene_0.initializeAndWait();

  PartDisplayer PD_0 = ((PartDisplayer) scene_0.getDisplayerManager().getDisplayer("Outline 1"));
  PD_0.initialize();

  PartDisplayer PD_1 = ((PartDisplayer) scene_0.getDisplayerManager().getDisplayer("Geometry 1"));
  PD_1.initialize();

  SceneUpdate sceneUpdate_0 = scene_0.getSceneUpdate();
  HardcopyProperties hardcopyProperties_0 = sceneUpdate_0.getHardcopyProperties();
  hardcopyProperties_0.setCurrentResolutionWidth(1506);
  hardcopyProperties_0.setCurrentResolutionHeight(618);
  scene_0.resetCamera();

  sim_0.saveState("D:\\STAR\\Venturi.sim");
 }

 private void execute1() {

  Simulation sim_0 = getActiveSimulation();

  MeshManager MM_0 = sim_0.getMeshManager();
  Region region_0 = sim_0.getRegionManager().getRegion("fluid");
  MM_0.convertTo2d(1.0E-18, new NeoObjectVector(new Object[] {region_0}), true);

  Scene scene_0 = sim_0.getSceneManager().getScene("Geometry Scene 1");
  CurrentView currentView_0 = scene_0.getCurrentView();
  currentView_0.setInput(new DoubleVector(new double[] {0.0, 0.0, 0.0}), 
    new DoubleVector(new double[] {0.0, 0.0, 1.0}), 
    new DoubleVector(new double[] {0.0, 1.0, 0.0}), 1.143640, 0, 30.0);
  scene_0.resetCamera();

  Region region_1 = sim_0.getRegionManager().getRegion("fluid 2D");
  region_1.setPresentationName("FLUID");

  Boundary BN_0 = region_1.getBoundaryManager().getBoundary("Default_Boundary_Region");
  Boundary BN_1 = region_1.getBoundaryManager().getBoundary("cyclic 2");
  MM_0.combineBoundaries(new NeoObjectVector(new Object[] {BN_0, BN_1}));
  MM_0.splitBoundariesByAngle(89.0, new NeoObjectVector(new Object[] {BN_0}));
  BN_0.setPresentationName("Axis");

  Boundary BN_2 = region_1.getBoundaryManager().getBoundary("Default_Boundary_Region 2");
  BN_2.setPresentationName("Outlet");

  Boundary BN_3 = region_1.getBoundaryManager().getBoundary("Default_Boundary_Region 3");
  BN_3.setPresentationName("Inlet");

  Boundary BN_4 = region_1.getBoundaryManager().getBoundary("Default_Boundary_Region 4");
  BN_4.setPresentationName("Wall");

  PhysicsContinuum Cm_0 = ((PhysicsContinuum) sim_0.getContinuumManager().getContinuum("Physics 1"));

  sim_0.getContinuumManager().remove(Cm_0);

  PhysicsContinuum Cm_1 = ((PhysicsContinuum) sim_0.getContinuumManager().getContinuum("Physics 1 2D"));

  Cm_1.setPresentationName("Physics 1");

  Cm_1.enable(SteadyModel.class);
  Cm_1.enable(SingleComponentLiquidModel.class);
  Cm_1.enable(SegregatedFlowModel.class);  
  Cm_1.enable(ConstantDensityModel.class);
  
  Cm_1.enable(TurbulentModel.class);
  Cm_1.enable(RansTurbulenceModel.class);
  Cm_1.enable(ReynoldsStressTurbulence.class);
  ReynoldsStressTurbulence RSM_0 = Cm_1.getModelManager().getModel(ReynoldsStressTurbulence.class);
  Cm_1.disableModel(RSM_0);

  Cm_1.enable(KOmegaTurbulence.class);
  Cm_1.enable(SstKwTurbModel.class);
  Cm_1.enable(KwAllYplusWallTreatment.class);
  
  sim_0.saveState("D:\\STAR\\Venturi.sim");
 }
}

Field Functions in STAR-CCM+

public class CreateUserFieldFunctions extends StarMacro {
  public void execute() {
    execute0();
  }
  private void execute0() {
    Simulation sim_0 = getActiveSimulation();

  UserFieldFunction uFF_0 = simulation_0.getFieldFunctionManager().createFieldFunction();
  uFF_0.getTypeOption().setSelected(FieldFunctionTypeOption.SCALAR);
  uFF_0.setPresentationName("R1");
  uFF_0.setFunctionName("R1");
  uFF_0.setDefinition("0.50");
	
  UserFieldFunction uFF_1 = sim_0.getFieldFunctionManager().createFieldFunction();
  uFF_1.getTypeOption().setSelected(FieldFunctionTypeOption.SCALAR);
  uFF_1.setPresentationName("Radius");
  uFF_1.setFunctionName("Radius");
  uFF_1.setDefinition("sqrt(($$Position[0]*$$Position[0])
    +($$Position[1]*$$Position[1]))");
  }
} 

Scripting in ANSA

ANSA uses Python as scripting and automation capabilities.
import os
import ansa
#from ansa import *

from ansa import base
def openFile():
	base.Open("C:/Users/myFile.ansa")

#Collect sets for different areas
deck = ansa.constants.LSDYNA
set1 = ansa.base.PickEntities(deck,("SET",))
parts = base.PickEntities(deck, ("SECTION_SHELL","SECTION_SOLID",))
set2 = base.CreateEntity(deck, "SET", {'Name' : "SetName", })
set3 = base.CollectEntities(deck, None, "__PROPERTIES__", )

def printPIDname():
	deck = constants.OpenFOAM  #NASTRAN, FLUENT, STAR, LSDYNA
	pid_list = base.collecEntities(deck, none, "PSHELL", False, True)
	#pid_list = base.collecEntities(deck, none, "__PROPERTIES__", False, True)
	for pid in pid_list:
		print(pid._name)
		oldPID = pid._name
		if "grille" in oldPID:
			newPID = "po_"+oldPID
			base.ReplaceProperty(oldPID, newPID)
		#subifm($,'oldPID','newPID')
		
def openMultipleFiles():
    #Select multiple files
	files = utils.SelectOpenFileIn('C:/Users/XYZ', 1)
	i = 1
	for f in files:
		print("File Number {1} is {2}:", i, f)
		#Opening the file
		ansa.base.Open(f) 
		i = i + 1
#------------------------------------------------------------------------------
#Print all PID and their names
import ansa
from ansa import *

idList = []
nameList = []
def main():
	deck = constants.LSDYNA
	pName = base.CollectEntities(deck, None, "__PROPERTIES__", False, True)
	for i in part_name:
		idList.append(i._id)
		nameList.append(i._name)
        pass
main()
mergeList = list(zip(idList, nameList))
for i in mergeList:      
    print(i)
	if __name__ == '__main__':
		main() 

Scripting in CFX and CFD-Post

A CCL CFX Command Language file required for scripting and automation in CFX is as follows. This file can also be used to set orthotropic thermal conductivity which is otherwise not possible through GUI. PERL statements can be directly embedded in CCL syntax. CCL syntax starting with 'gt;' is execution statement. The PERL statements start with '!'. \ is the line continuation character and lists are separated by comma. CFD-Post session file have extension .cse (CFX SEssion) and .cst (CFX STate).
dP = massFlowAve(Pressure)@inlet – massFlowAve(Pressure)@outlet
Pv = 0.5 * areaAve(Density)@Inlet * areaAve(Velocity)@Inlet^2
areaAve(p)@Inlet - area-weighted average of 'pressure' on the boundary named 'Inlet'
area()@REGION:Inlet - area of a 2D mesh region named 'Inlet' belonging to domain REGION. area_x()@Inlet is area projected in direction 'X'.
massFlow()@Inlet: mass flow rate through 'Inlet'. Add multiple zones separated by space. e.g. massFlow()@Out1 Out2 Out3
>calculate area, Inlet, - calculates the area of the locator 'Inlet'. Note that adding the comma after 'Inlet' removes the axis specification.
@Xlocs = (0.05, 0.10, 0.15, 0.20) - define a list in PERL, $Xlocs[$i] - accesss a member in the list.
volumeInt(Density)@Tank - calculate mass of luid in volume named 'Tank'

Print mass flow rate, area and area-average velocity on single line: here 'front' is the name of the boundary.

!print("front: Mass Flow Rate [kg/s] = 10%5f, Area [m^2] = %10.6f, Area-Avg-Velocity [m/s] = %10.2f", massFlow("front"), area("front"), areaAve("Velocity", "front"), "\n");

Example PERL script - use it in command editor, the output would be printed in CFD-Post terminal.

! ($MFinlet, $MFunit) = evaluate("massFlow()\@Inlet");
! printf (Mass Flow at Inlet "%10.5f [$MFunit] \n", $MF01);

! for ($i = 1; $i <= 8; $i++) {
!  if ($i < 10) { 
!   $i = '0'.$i; 
!  }
!
!  ($ARi, $ARunit) = area()@OUTLET_.$i;
!  ($MFi, $MFunit) = massFlow("OUTLET_.$i");
!  printf("OUTLET_.$i = %10.5f [$ARunit], MF = %10.5f [$MFunit] \n", $ARi, $MFi);
! }

Write output or results of function calculators to a FILE.

! $AvQ=areaAve("Wall Heat Flux", "WALL_CYL");
! open(RESULT, ">Output.dat");
! print RESULT "-------------------------------------------------\n";
! print RESULT "$AvQ\n";
! print RESULT "-------------------------------------------------\n";
! close(RESULT); 

Create a PLANE in CFD-Post


Create a pressure contour on PlaneYZ created earlier.


Set Camera Views, Show/Hide Contours and save hardcopies

# Sending visibility action from ViewUtilities
>show /CONTOUR:ContourPlaneYZ, view=/VIEW:View 1

# Sending visibility action from ViewUtilities
>hide /PLANE:PlaneYZ, view=/VIEW:View 1

>setcamera viewport=1, camera=-X
HARDCOPY:
  Antialiasing = On
  Hardcopy Filename = Orifice_Walled_Duct_HighTI_001.png
  Hardcopy Format = png
  Hardcopy Tolerance = 0.0001
  Image Height = 600
  Image Scale = 100
  Image Width = 600
  JPEG Image Quality = 80
  Screen Capture = Off
  Use Screen Size = On
  White Background = On
END
>print 

CCL and PERL are case sensitive.

COMMAND FILE:
  CFX Pre Version = 12.1
END
# Define variables in a PERL file and include with 'require' statement
! require "VarCFX_Pre.pl";
>load mode=new
>update

>gtmImport filename=$FCFX5, type= Generic, genOpt= -n, units=mm, \
nameStrategy=$Name
> update
>writeCaseFile filename=$CASE
> update

FLOW: Flow Analysis 1
  &replace   SOLUTION UNITS:
    Angle Units = [rad]
    Length Units = [m]   #Options: [cm], [mm], [in], [ft], [yd], [mile]
    Mass Units = [kg]    #Options: [g], [lb], [slug], [tonne]
    Solid Angle Units = [sr]
    Temperature Units = [K]  #Options; [R]
    Time Units = [s]     #Options: [min], [hr], [day], [year]
  END # SOLUTION UNITS:
END # FLOW:Flow Analysis 1
> update
# ---------------------------------------------------------------------+
LIBRARY:
 CEL:
  EXPRESSIONS:
   CpAir=1005.6 [J kg^-1 K^-1] + 5.6E-3 [J kg^-1 K^-2] * T
  END
 END
END
> update

LIBRARY:
 CEL:
  EXPRESSIONS:
   kAir = -3.9333E-4[W m^-1 K^-1] + 1.0184E-4 [W m^-1 K^-2]*T \
    -4.8574E-8 [W m^-1 K^-3]*T*T + 1.5207E-11 [W m^-1 K^-4]*T^3
  END
 END
END
> update

LIBRARY:
 CEL:
  EXPRESSIONS:
   MuAir=1.72E-5 [kg m^-1 s^-1] *(T / 293 [K])^0.742
  END
 END
END
> update

LIBRARY:
 CEL:
  EXPRESSIONS:
   AvHeatFlux=areaAve(Wall Heat Flux )@REGION:$WallName
  END
 END
END
> update
# ---------------------------------------------------------------------+

Set Boundary Conditions and Solver Parameters

FLOW: Flow Analysis 1 &replace OUTPUT CONTROL: MONITOR OBJECTS: MONITOR BALANCES: Option = Full END # MONITOR BALANCES: MONITOR FORCES: Option = Full END # MONITOR FORCES: MONITOR PARTICLES: Option = Full END # MONITOR PARTICLES: MONITOR POINT: Mon1 Expression Value = VF Option = Expression END # MONITOR POINT:Mon1 MONITOR RESIDUALS: Option = Full END # MONITOR RESIDUALS: MONITOR TOTALS: Option = Full END # MONITOR TOTALS: END # MONITOR OBJECTS: RESULTS: File Compression Level = Default Option = Standard END # RESULTS: END # OUTPUT CONTROL: END # FLOW:Flow Analysis 1 > update # ---------------------------------------------------------------------+ > writeCaseFile > update >writeCaseFile filename=$DEF, operation=start solver interactive # operation="write def file" or "start solver batch" > update

Post-processing statements in PERL


DOS Scripts

'DOS' (the Disk Operating System) is used to describe cmd (ther command terminal). In Windows OS, DOS commands are stored in a text file with extension *.bat (BATch) files. These files can be used to run programs in batch (non-GUI) mode and automated repeated tasks. By default, a batch file will display its command as it runs. Command "echo off" turns off the display for the whole script, except command itself. Sign '@' in front makes the command apply to itself as well.

  1. The redirect operator > directs the output to specfied location (terminal, file...). >> is used to append the output to an existing content
  2. The command line arguments can be called through the variables %1, %2, %3 and so on
  3. Variables: set /A X=10, echo %X%, SET /A c = %a% + %b% - variable is assigned using 'set' command and value is accessed using %...% operator

Run multiple commands one after another in DOS Terminal: Conditional Execution

  1. The conditional execution & starts next task after execution of previous task has (whether with error or with success) finished: e.g. ocrmypdf --output-type pdf --skip-text -l hin+eng In-1.pdf Out-1.pdf & ocrmypdf --output-type pdf --skip-text -l hin+eng In-2.pdf Out-2.pdf
  2. The conditional execution & starts next task after execution of previous task has successfully finished: e.g. ocrmypdf --output-type pdf --skip-text -l hin+eng In-1.pdf Out-1.pdf && ocrmypdf --output-type pdf --skip-text -l hin+eng In-2.pdf Out-2.pdf
  3. Additionally, the double pipe || symbols start the next command if the previous command fails
  4. Alternatively, add all the commands line by line in a batch file, and save the file as say batchRuns.bat. Execute that batch file which would run all the commands sequentially in the order they are stored in the file. A batch file executes a command and waits until the command is finished, then runs the next command. Use start to start the batch file: e.g. start "" batchRuns.bat - The empty pair of double-quote marks is for the "Title" that will be shown in the title bar of the command window that start command will open.

File Seach in Windows 10

From Command Line - search files bigger than 10 MB --- forfiles /P F:\DataFiles\XYZ /M * /S /C "cmd /c if @fsize GEQ 10485760 echo @path > bigFiles.log" --- note that it creates files bigFiles.log in each sub-directory of parent directoty [F:\DataFiles\XYZ in this case]

Here GEQ = ≥, 1kB = 1,024 bytes -- 1 MB = 10,48,576 byts -- 1 GB = 1,07,37,41,824 bytes. forfiles takes following arguments: /P "pathname" - Specifies the path from which to start the search. By default, searching starts in the current working directory. /M "searchmask" - Searches files according to the specified search mask. The default searchmask is *. /S - Instructs the forfiles command to search in subdirectories recursively. /C "command" - Runs the specified command [should be wrapped in double quotes] on each file. Default command is "cmd /c echo @file".

File Search by Size in Windows 10

The options and range of file size which is seached is summarized as follows:
  1. small: 16kB ~ 1 MB
  2. medium: 1 ~ 128 MB
  3. large: 128 MB ~ 1 GB
  4. huge: 1 ~ 4 GB
  5. gigantic: > 4 GB
  6. size: > 100MB can be used to each for files having size > 100 MB. Similarly, size: > 50MB < 80MB can be used to find the files having size in a specified range.
  • % is used to refer to a variable: e.g. %f IN (in*.f) where %f refers to file names matching 'in*.f'
  • REM (REMark) or :: is used for comments. DOS commands are not case-sensitive
  • Line contunuation: You may break up long lines of code with the caret ^. Put it at the end of a line, next line must have space at the begining
  • dir /T:W >> list.txt: write files of the current folder into file list.txt
  • dir /T:W C:\commands.docx: Get the last modified time for the file 'C:\commands.docx'
  • dir /T:W -> Get modified date/time for all files and folders in the current directory
  • dir /T:W /A:-D -> Get modified date/time only for files in the current directory (exclude folders)
  • Using forfiles command we can get modified date/time for all files in a directory: forfiles /C "cmd /c echo @file @fdate @ftime"
  • Restrict the command only to certain files using * command. E.g. get modified time/date only for pdf files: forfiles /M *.pdf /C "cmd /c echo @file @fdate @ftime"
  • List the content of folder and its sub-folders: dir C:\XYZ /ad /b /s > List.log
  • rmdir /q /s "%%I" -> it will delete directories quietly and removes all files, sub-folders and the directory itself
  • Calls another batch file and returns control to the first when done: CALL C:\NEW.bat
  • To echo special characters, precede them with a caret: ECHO ^<
  • Spliting strings: "tokens=1-5 delims=/ " - How many tokens the incoming data (in this case the date) will be broken into. 1-5 is five different tokens. The 'delims' argument is short for delimiters and is what is used to break up the date, in this example the / (forward slash) and a space (space before the quote)
  • for /f "tokens=1-5 delims=/ " %%d in ("%date%") do rename "hope.txt" %%e-%%f-%%g.txt, use the date command within the for command to extract the current date and use that data to rename the file.

EAMPLES

Merge Files:
FOR %f IN (in*.f) 
 DO 
  type %f >> ..\merge.txt & echo. >> ..\merge.txt

@echo off 
set list=1 2 3 4 
(for %%a in (%list%) do ( 
   echo %%a 
))

Open many files using NOTEPAD:
cd C:\Test
for %X in (*.f) 
 do 
   notepad %X

Create a file name based on current date and time:
Set Mn = %DATE:~7,2%
Set Yr = %DATE:~10,4%
Set Hr = %TIME:~0,2%
Set Mi = %TIME:~3,2%
dir "C:\XYZ"  /-C /O:GN /Q /S /T:A > "%Day%-%Mn%-%Yr% %Hr%-%Mi%.log"

Use of CONDITIONAL statements:
@echo off
if exist c:\XYZ goto exists
  echo Directory not found
  pause
goto end
:exists
  echo The directory exists
  echo .
:end
  Set FilePath=%FilePath%\%Day%
  IF NOT EXIST %FilePath% MKDIR %FilePath%
  @echo off

Python Code to create Summary of a Text File

Most of the programs such as ANSYS FLUENT and STAR-CCM+ have a well-defined structure to report summary of the set-up file. This Python code can be used to summary the lines containing specific keyword. The code has been tested on this sample text file.


Scheme examples from web such as cookbook.scheme.org, schemers.org....

Find first occurrence of an element in a list

(define (list-index fn list)
  (let iter ((list list) (index 0))
    (if (null? list) -1
      (let ((item (car list)))
        (if (fn item)
          index
          (iter (cdr list) (+ index 1))
        )
      )
    )
  )
)

Remove duplicate (repeat) entries from a list which are adjacent to each other

(define (delete-adjacent-duplicates xs)
  (let loop ((prev-pair #f) (xs xs) (new-list '()))
    (if (null? xs) (reverse new-list)
       (loop xs
          (cdr xs)
          (let ((x (car xs)))
            (if (and prev-pair (equal? x (car prev-pair)))
               new-list
               (cons x new-list)
            )
          )
       )
    )
  )
) 
(delete-adjacent-duplicates '(1 2 3 1 1 4 5 5)) = (1 2 3 1 4 5)

Find substring in string: this will work only is (char?) is defined.

(define (string-find haystack needle . rest)
  (let ((start (if (null? rest) 0 (car rest))))
    (let* ((haystack-len (string-length haystack))
           (needle-len (string-length needle))
           (start 0))
      (let loop ((h-index start)
                 (n-index 0))
        (let ((h-char (string-ref haystack h-index))
              (n-char (string-ref needle n-index)))
          (if (char=? h-char n-char)
            (if (= (+ n-index 1) needle-len)
               (+ (- h-index needle-len) 1)
               (loop (+ h-index 1) (+ n-index 1))
            )
            (if (= (+ h-index 1) haystack-len) #f
               (loop (+ h-index 1) 0)
            )
          )
        )
      )
    )
  )
)
(string-find input search)
(define (list? x)
  (if (equal? (length x) 0) #f)
  (if (> (length x) 0) #t)
) 
(list? '2) - error, (list? '(2 3)0 = #t, (list? '()) = #f.

Examples from stackoverflow.com/ ... /searching-and-replacing-n-element-on-list-scheme: the keyword list has been replaced with xlst.

(define (find-replace a b xlst)
  (cond
    ;Start with a list. If it's empty, leave it
    ((null? xlst) '())
    ;If the first element is a list, call function recursively. If the first 
    ;element is equal to what your searching for, cons the replacement onto a 
    ;recursive call of your function on the rest of the list...keep searching
    ((list? (car xlst)) 
       (cons (find-replace a b (car xlst)) (find-replace a b (cdr xlst)))
    )
    ((eq? (car xlst) a) (cons b (find-replace a b (cdr xlst))))
    ;If none of the earlier conditions are true, cons the first element on to
    ;a recursive call of your function for the rest of the list
    (else
      (cons (car xlst) (find-replace a b (cdr xlst)))
    )
  )
)
Reference: The Little Schemer
(define atom?
  (lambda (x)
    (and (not (pair? x)) (not (null? x)))
  )
)

Substitute every occurrence of old with an occurrence of new. Note that this code will work only if (atom?) is defined which is not the case in all Scheme implementations.

(define subst-lst
  (lambda (new old l)
    (cond
       ((null? l) (quote ()))
       ((atom? (car l))
         (cond
           ((eq? (car l) old) (cons new
             (subst new old (cdr l)))
           )
           (else (cons (car l)
             (subst new old (cdr l)))
           ) 
         )
	  )
      (else (cons (subst new old (car l))
        (subst new old (cdr l)))
      )
    )
  )
) 
Some Examples from GitHub
(define (delete-n list n)
  (if (= n 0)
    (cdr list)
    (cons (car list) (delete-n (cdr list) (- n 1)))
  )
)

(define (insert-n list item n)
  (if (= n 0)
    (cons item list)
    (cons (car list) (insert-n (cdr list) item (- n 1)))
  )
)

(define (list-nth list n)
  (if (= n 0)
    (car list)
    (list-nth (cdr list) (- n 1))
  )
)

(define (replace-nth list n item)
  (if (= n 0)
    (cons item (cdr list))
    (cons (car list) (replace-nth (cdr list) (- n 1) item))
  )
)

(define (swap-item list m n)
  (let
    ( (a (list-nth list m)) (b (list-nth list n)) )
    ( replace-nth (replace-nth list m b) n a )
  )
)

Examples:
(swap-item (list 1 2 3 6) 2 3)
(replace-nth (list 3 2 9 2) 2 8)
(delete-n (list 1 2 3 4 5) 2)
(insert-n (list 1 2 3 4 5) 8 2)
(list-nth (list 1 2 3 4 5) 3) 

From the Book: Concrete Abstractions - An Introduction to Computer Science Using Scheme

Procedure that counts the number of elements in a list:
(define length
  (lambda (lst)
    (if (null? lst) 0
      (+ 1 (length (cdr lst)))
    )
  )
) 

Procedure that selects those elements of a given list that satisfy a given predicate:

(define filter
  (lambda (ok? lst)
    (cond ((null? lst) '())
      ((ok? (car lst))
        (cons (car lst) (filter ok? (cdr lst)))
      )
      (else
        (filter ok? (cdr lst)))
    )
  )
)
Example: (filter odd? (integers-from-to 1 15)) = (1 3 5 7 9 11 13 15)
Linux Commands and Utilities

Install a package (program): sudo apt install okular

Uninstall a package excluding dependent packages: sudo apt remove okular

Uninstall a package including dependent packages: sudo apt remove --auto-remove okular

Uninstall a package including configuration and dependent packages: sudo apt purge okular

Uninstall everything related to a package (recommended before reinstalling a package): sudo apt purge --auto-remove okular

Contact us
Disclaimers and Policies

The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all content.