The loading and solution phase starts with the /SOLU command. In this phase, you do the following tasks:
Other solution-related items - master DOF and gap conditions - are also defined in this phase.
Analysis types are generic and independent of discipline:
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.
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 . . . . . . . .
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,...)
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
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
"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
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 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
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
Inertia load commands are the same as at Revision 4.4.:
ACEL,OMEGA,DOMEGA,CGLOC,CGOMEGA,DCGOMG,IRLF
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,RTHreads temperature at time=5.78 from file THERMAL.RTH.
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
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
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 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 ANSYSThe script file and ANSYS input file may be kept in your home directory or its subdirectory.. qsub -q ANSYS.snake .
#@$-lt 20:00 #@$-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.
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 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/xxIf 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
Multiple load steps can be solved by three methods:
... Load data LSWRITE ----> File.S01 ! Load data LSWRITE ----> File.S02 ! Load data LSWRITE ----> File.S03 ! ... LSSOLVE
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)=0.0,0.8,7.2,8.5,9.3Then 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 *ENDDOThe 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.
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:
ANSYSoutput-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 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