8/11/17 Loading and Solution
Loading and Solution
Loading and Solution
The loading and solution phase starts with the /SOLU command. In this phase, you do the following tasks:
Define the analysis type and analysis options.
Apply loads
Initiate the solution
Specify load step options
Select Outputs
Other solution-related items - master DOF and gap conditions - are also defined in this phase.
Defining the analysis type and analysis options.
Analysis types are generic and independent of discipline:
Static (or steady-state)
Transient
Harmonic
Modal
Spectrum
Buckling
Substructuring
On menu mode, control panels are available to define analysis
type and analysis options. For non-menu mode, ANTYPE
command replaces KAN.
ANTYPE, STATIC (or 0)
TRANS (or 4)
MODAL (or 2)
etc.
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 1/9
8/11/17 Loading and Solution
Analysis Options
MODOPT ! Modal analysis options
TRNOPT ! Transient analysis options
HROPT ! Harmonic analysis options
BUCOPT ! Buckling analysis options
SSTIF ! Stress stiffening
NROPT ! Newton-Raphson options
Etc.
Preconditioned Conjugate Gradient (PCG) solver has been added as an alternate to the default frontal solver.
The PCG solver requires less file space but more memory than other solvers and is faster for larger
models(wavefronts > 1000). PCG is well-suited for problems with very large, sparse, symmetric matrices, such
as those encountered in magnetic field analysis.
/SOLUTION
ANTYPE,STATIC
EQSLV,PCG
........
Applying loads
There are six categories of loads, each with a generic set of commands:
Family Category
D ! DOF Constraints (displacements,temperatures,...)
F ! "FORCES" (forces,moments,heatflows,...)
SF ! Surface Loads (pressures,convections,...)
BF ! Body Loads (temperatures,heat generations,...)
ACEL ! Inertia Loads (accelerations,...)
LDREAD ! Coupled-Field Loads (thermal strain,...)
1. DOF constraints
DOF constraints available in each discipline:
Discipline Degree of Freedom ANSYS Label
Structural Translations UX,UY,UZ
Rotations ROTX,ROTY,ROTZ
Thermal Temperature TEMP
Magnetic Vector Potential AX,AY,AZ
Scalar Potential MAG
Electric Voltage VOLT
Fluid Velocities VX,VY,VZ
Pressure PRES
Turb. Kinetic Energy ENKE
Turb. Dissipa. Rate ENDS
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 2/9
8/11/17 Loading and Solution
DOF constraint commands:
Location Commands
Nodes D,DSYMM,DLIST,DDELE,DSCALE,DCUM
Keypoints DK,DKLIST,DKDELE
Lines DL,DLLIST,DLDELE
Areas DA,DALIST,DADELE
Transfer DTRAN,SBCTRAN
2. "FORCE"
"FORCE" available in each discipline:
Discipline "Force" ANSYS Label
Structural Forces FX,FY,FZ
Moments MX,MY,MZ
Thermal Heat Flow Rate HEAT
Magnetic Current Segments CSGX,CSGY,CSGZ
Magnetic Flux FLUX
Electric Current AMPS
Fluid Fluid Flow Rate FLOW
Heat Flow Rate HEAT
"FORCE" load commands:
Location Commands
Nodes F,FLIST,FDELE,FSCALE,FCUM
Keypoints FK,FKLIST,FKDELE
Transfer FTRAN,SBCTRAN
3. Surface loads
Surface loads available in each discipline:
Discipline Surface Load ANSYS Label
Structural Pressure PRES
Thermal Convection CONV
Heat Flux HFLUX
Magnetic Maxwell Surface MXWF
Electric -none- -none-
Fluid Fluid-Structural FSI
Impedance IMPD
Convection CONV
Heat Flux HFLUX
All Superelement SELV
Load Vector
Surface load commands:
Location Commands
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 3/9
8/11/17 Loading and Solution
Nodes SF,SFLIST,SFDELE,SFSCALE,SFCUM,SFFUN,
SFGRAD
Elements SFE,SFELIS,SFEDEL,SFBEAM,SFFUN,SFGRAD
Lines SFL,SFLLIST,SFLDELE,SFGRAD
Areas SFA,SFALIST,SFADELE,SFGRAD
Transfer SFTRAN,SBCTRAN
e.g. NSEL,...
SF,ALL,PRES,5000 ! Pressure on all selected nodes
4. Body loads
Body loads available in each discipline
Discipline Body Load ANSYS Label
Structural Temperature TEMP
Fluence FLUE
Thermal Heat Generation Rate HGEN
Magnetic Current Density JS
Virtual Displacement MVDI
Electric -none- -none-
Fluid Heat Generation rate HGEN
Body load commands:
Location Commands
Nodes BF,BFLIST,BFDELE,BFSCALE,BFCUM,BFUNIF
Elemnets BFE,BFELIS,BFEDEL,BFESCAL,BFECUM
Keypoints BFK,BFKLIST,BFKDELE
5. Inertia load
Inertia load commands are the same as at Revision 4.4.:
ACEL,OMEGA,DOMEGA,CGLOC,CGOMEGA,DCGOMG,IRLF
6. Coupled-field load
Coupled-field loads are applied using the new command LDREAD which reads data from the results file and
applies them as loads. For example,
LDREAD,TEMP,,,5.78,,,THERMAL,RTH
reads temperature at time=5.78 from file THERMAL.RTH.
Displaying loads
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 4/9
8/11/17 Loading and Solution
Applied loads may be displayed with the following three commands:
/PBC ! For Ds and Fs
/PSF ! For SFs
/PBF ! For BFs
For examples:
/PBC,U,,1 ! For displacements
/PBC,F,,1 ! For forces
/PBC,all,,a ! For all appropriate symbols
/PBC,ACEL,,1 ! Applied accelerations
/PSF,PRES,NORM,1
/PBF,TEMP,,1
Initiating the solution
SOLVE is the command that initiates the solution; it reads data from database to calculate solution and writes
results to database and also to the results file.
This is the actual computing portion of the analysis, and a complex ANSYS job often requires considerable
amount of CPU time. It is advisable that you save the database prior to executing the SOLVE command ( with
"SAVE, filename,db") and exit the ANSYS program. Next, create a batch submit file as the following:
# @$-lt 20:00
# @$-lw 32mb
# @$-eo
# @$-me
ANSYS <<'EOT'
/BATCH
/RESUME,<Filename>,db
/SOLUTION
SOLVE
FINISH
EXIT
'EOT'
This batch job can then be submitted to the tiber with the "qsub" command:
qsub batch-submit-file-name
Running an ANSYS job on the IBM RS6000 Cluster
The IBM RS6000 cluster machines are to be used as back-end machines, though users can login to the hudson
and interactively run ANSYS. Users are requested to run ANSYS interactively only for preparing the ANSYS
commands in /PREP7 and for reviewing the results in /POST1 or /POST26. The CPU intensive solution phase
must be run in batch mode. If users abuse the trust and run the CPU intensive solution phase that makes hudson
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 5/9
8/11/17 Loading and Solution
unavailable to other users, severe restrictions will be imposed to all ANSYS users. As a rule of thumb, if the
SOLVE takes more than 3 minutes of CPU time, run it in batch.
Two of the RS6000s, snake and pecos, have been designated to run ANSYS batch jobs. The total size of files
created by ANSYS cannot exceed 2 GB in /tmp in pecos, while it is possible to exceed 2 GB in snake by
assigning files to two directories, /tmp and /wrk. Thus an ANSYS job that may create a total file size greater than
2 GB must run on snake. Users may follow the examples below to prepare an ANSYS batch script file on the
hudson and submit it to the pecos or the snake by the qsub command with "-q ANSYS" or "-q ANSYS.snake".
The ANSYS queue will run ANSYS on either pecos or snake, while ANSYS.snake will run ANSYS only on
snake.
qsub -q ANSYS .
qsub -q ANSYS.snake .
The script file and ANSYS input file may be kept in your home directory or its subdirectory.
Example: An ANSYS batch script to run on an IBM RS6000:
#@$-lt 20:00
#@$-lw 32mb
#@$-eo
#@$-me
date
mkdir /tmp/tang
cd /tmp/tang
cp /user/marge/spring* .
/usr/local/bin/ANSYS <<'EOT'
/BATCH
! /assign,tri,spring,tri,/wrk/tang/ !!! Only for ANSYS.snake with
! /assign,emat,spring,emat,/wrk/tang/ !!! total file size > 2 GBs
/input,spring,prep
/input,spring,ldso
/input,spring,post
/input,spring,opt
/input,spring,full
/exit
'EOT'
ls -l /tmp/tang !!! Check files created created by ANSYS
! ls -l /wrk/tang !!! On snake only
mv *.rst /tiber/support/tang/ANSYS/.
mv *.db /tiber/support/tang/ANSYS/.
rm /tmp/tang/* !!! Clean up your files to provide file space
! rm /wrk/tang/* !!! for next job to use.
Moving files from pecos to your home directory
The ANSYS program creates several output files that are in the order of tens of megabytes in pecos temporary
file space. These files are not interactively accessible because pecos is not directly accessible to user, but users
can use rsh command to browse these files:
rsh pecos ls -l /tmp/usrname
rsh pecos cat /tmp/usrname/filename.out
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 6/9
8/11/17 Loading and Solution
rsh pecos rm /tmp/usrname/xx.
To copy a file from /tmp/usrname on pecos to somewhere in your tiber directory, you need to have
hudson.nist.gov in your tiber .rhosts and then use:
rcp pecos:/tmp/usrname/xx subdir/xx
If your home directory is on hudson and the file is too large to keep on hudson, specify a full pathname to your
tiber directory:
rcp pecos:/tmp/marge/xx /tiber/nist/marge/xx
Specifying load step options
Multiple load steps can be solved by three methods:
Load step file method
Array parameter method
Multiple SOLVE method
In the load step file method, each load step is written(LSWRITE) to a different file - File.S01, File.S02,
File.S03,..., etc. The action command LSSOLVE reads in these step files sequentially and initiates the solution
for each step.
...
Load data
LSWRITE ----> File.S01
!
Load data
LSWRITE ----> File.S02
!
Load data
LSWRITE ----> File.S03
!
...
LSSOLVE
Specifying load step options
New LSCLEAR command clears loads and load step options in the database, while LSREAD and LSDELE
reads and deletes a load step file, respectively.
With the array parameter method, array parameters of type TABLE are used to define load versus time:
*DIM,LOAD,TABLE,5
LOAD(1)=0.0,560.0,560.0,238.5,0.0
LOAD(1,0)=0.0,0.8,7.2,8.5,9.3
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 7/9
8/11/17 Loading and Solution
Then use a do-loop to apply the load and solve it:
DTIME=0.01 ! Time step size
*DO,TIMEV,1.0E-6,5.8,DTIME
TIME,TIMEV
F,293,FY,LOAD(TIMEV)
SOLVE
*ENDDO
The multiple SOLVE method defines load data, issues SOLVE; changes load data, issues SOLVE; and so on.
This method is better suited for batch mode than for interactive mode.
Selecting Outputs
New output controls separate print and post:
OUTPR,Item,FREQ,.....
OUTRES,Item,FREQ,....
If you have already prepared an ANSYS input file with PREP7, at the system prompt, you can redirect the input
file to ANSYS and run it in the background mode:
ANSYS output-file-name &, or
/input,input-file-name,ext,dir within ANSYS.
/SOLU ! Enter the SOLUTION processor
ANTYPE,STATIC ! Static (steady-state) analysis
TUNIF,0 ! Initial Uniform Temp = 0
KBC,1 ! Step loading
CNVTOL,TEMP,1.0,1.0E-6
CNVTOL,HEAT,1.0,1.0E-6
/FORMAT,,E,14,6
PI=3.1415927
NSEL,S,,,91,95 ! Select node 91-95, Y=4.0-4.2
F,ALL,HEAT,10/PI ! Constant heat flow rate per radian
! Total heat load = 10000 nW
NSEL,S,LOC,Y,-3.5
D,ALL,TEMP,0 ! Base Temperature
ALLSEL
OUTPR,NSOL,1
OUTRES,NSOL,1 ! Write node solutions to the result file
/PBC,HEAT,1 ! Show heat rate load
/PBC,TEMP,1 ! Show boundary temp load
EPLOT
AUTOTS,OFF ! Turn off automatic load-stepping
NSUBST,20 ! Only 1 substep is sufficient
SOLVE
SAVE
FINISH ! End of SOLUTION process
/POST1 ! Enter postprocess
* ASK,LS,'Load Step to Display LS:',1
SET,LS,LAST
/TITLE,TEMPERATURE CONTOUR PLOT
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 8/9
8/11/17 Loading and Solution
NSEL,S,,,1,150
PLNSOL,TEMP ! Display temperature
/SOLUTION ! Enter the SOLUTION processor
ANTYPE,TRANS ! Set analysis type = transient
TUNIF,0 ! Initially uniform temp = 0
TIMINT,ON ! Transient effect considered
KBC,1 ! Step loading
/FORMAT,,E,14,6
PI=3.1415927
TIME,100 ! Total of 100 sec
DELTIME,600 ! What does it mean?
AUTOTS,OFF ! Turn off automatic load-stepping
NSUBST,400 ! Use 400 substeps - 4 steps per sec
NSEL,S,,,91,95 ! Select node 91-95, i.e., Y = 4.0 - 4.2
F,ALL,HEAT,10.0/PI ! Constant heat flow rate per radian
! Total of 10000 nW applied
NSEL,S,LOC,Y,-3.5
D,ALL,TEMP,0
ALLSEL
/PBC,HEAT,1 ! Show heat load
/PBC,TEMP,1 ! Show temperature load
EPLOT
OUTPR,NSOL,4
OUTRES,NSOL,4 ! Write all solutions to the result file
*DO,TIMEVAL,BGNTIME,ENDTIME,DELTIME
TIME,TIMEVAL
SOLVE
*ENDDO
FINISH ! End of SOLUTION process
*ASK,LS,'Load Step to Display LS:',1
SET,LS,LAST
/POST26 ! Enter postprocess time history
/TITLE,TEMPERATURE CONTOUR PLOT
PLNSOL,TEMP ! Display temperature
NSOL,2,1,TEMP,Node-1
NSOL,3,11,TEMP,Node-11
NSOL,4,41,TEMP,Node-41
NSOL,5,71,TEMP,Node-71
NSOL,6,91,TEMP,Node-91
NSOL,7,101,TEMP,Node-101
PRNSOL,2,3,4,5
Hai Tang, last updated December 12, 1995
math.nist.gov/mcsd/savg/tutorial/ansys/ldsolutn/index.html 9/9
