Creating Parameters in Mechanical for use in Equations
-
-
Hello Community,
I understand well how to generate input Parameters in DesignModeler to alter geometry and generate output Parameters in Mechanical in order to setup a Design Study.
I want to know if it is possible to use an input Parameter in an equation for an Acceleration load.
Regards,
Peter
-
-
-
-
@peteroznewman I am looking for an alternative way, to automate the process. Let me know if this looks plausible
1. Assume a structural transient problem has been set up in ANSYS Workbench 19.1 and has been solved and deformation probe results are in the tabular data.
2. From Workbench>Transient module>Mechanical>Tools>Write input file (input.dat).
3. Write a Command snippet to write a text file to HDD of the tabular data (Amplitude vs time) in Transient>Solution (output.dat)
4. Open the "input.dat" in MATLAB, edit the row and change the frequency, write new output.dat, perform data processing in MATLAB, repeat in a loop.
If this sounds plausible, how could I write the command snippet for this, any template or pointers to refer?
-
Punnung, your approach is very feasible to get a large number of runs at different frequencies. The frequency is easily found in the input.dat data file. You could write out a large number of input_.dat files from matlab where is the sequence number of the file, one for each frequency.
There is a Windows batch file command line to start the solver that I can provide that defines the name of the input file and the name of the output file. That Windows batch file can have as many lines in it as the number of frequencies you want results. I did this once on a Linux system with a script, and was pleased that the next line of the script didn't get executed until the previous solve completed. I hope it works the same on Windows.
All you need is the command snippet to write the output of the Probe to a text file. I hope someone on the forum can provide that since I am a beginner at writing APDL code. They might also put in the lines for a for loop to have APDL loop through the frequencies and write out a unique file for each loop, then you don't need to create the Windows batch file.
I wrote out a ridiculously coarse mesh to get a very short input.dat file so I could block quote that below and also attach in the zip file. I found the frequency of 9.44 on two of the lines that I emphasized with bold text. Not sure why it appears twice. That is the number that you want to loop through a range of values.
/batch
/config,noeldb,1 ! force off writing results to database
*get,_wallstrt,active,,time,wall
! ANSYS input file written by Workbench version 19.1 RELEASE
! File used for geometry attach: E:ansysdatastudentcommunityPunnangSupport_ANSYSFull_transient__Parametric_Peter_filesdp0SYSDMSYS.agdb
/title,Full_transient__Parametric_Peter--Transient (E5)
! ****** Begin Custom Load Command Snippet ******
/COM, ACT Extensions:
/COM, MechanicalDropTest, 2.0
/COM, f0fd899f-9d88-4f46-8cf1-36bf5c218d65, wbex
/COM,
! ****** End Custom Load Command Snippet ******
*DIM,_wb_ProjectScratch_dir,string,248
_wb_ProjectScratch_dir(1) = 'E:ansysdatastudentcommunityPunnangSupport_ANSYSFull_transient__Parametric_Peter_filesdp0SYS-4MECH'
*DIM,_wb_SolverFiles_dir,string,248
_wb_SolverFiles_dir(1) = 'E:ansysdatastudentcommunityPunnangSupport_ANSYSFull_transient__Parametric_Peter_filesdp0SYS-4MECH'
*DIM,_wb_userfiles_dir,string,248
_wb_userfiles_dir(1) = 'E:ansysdatastudentcommunityPunnangSupport_ANSYSFull_transient__Parametric_Peter_filesuser_files'
/com,--- Data in consistent BIN units. See Solving Units in the help system for more information.
/units,BIN
/nopr
/wb,file,start ! signify a WB generated input file
/prep7
! Turn off shape checking because checks already performed inside WB mesher.
! See help system for more information.
SHPP,OFF,,NOWARN
/nolist
etcon,set ! allow ANSYS to choose best KEYOP's for 180x elements
/com,*********** Nodes for the whole assembly ***********
nblock,3,,74
(1i9,3e20.9e3)
1 5.549449106E+00 4.937399556E+00 7.070417328E+00
2 5.549449106E+00 4.937399556E+00 8.070417328E+00
3 7.163622334E+00 4.937399556E+00 7.070417328E+00
4 7.163622334E+00 4.937399556E+00 8.070417328E+00
5 -2.127716248E+00 4.937399556E+00 7.070417328E+00
6 -2.127716248E+00 4.937399556E+00 8.070417328E+00
7 -2.127716248E+00 4.945273572E+00 7.070417328E+00
8 -2.127716248E+00 4.945273572E+00 8.070417328E+00
9 -5.135430201E-01 4.945273572E+00 7.070417328E+00
10 -5.135430201E-01 4.945273572E+00 8.070417328E+00
11 -1.320629634E+00 4.945273572E+00 7.070417328E+00
12 -1.320629634E+00 4.945273572E+00 8.070417328E+00
13 5.549449106E+00 4.945273572E+00 7.070417328E+00
14 5.549449106E+00 4.945273572E+00 8.070417328E+00
15 4.969556676E-01 4.945273572E+00 7.070417328E+00
16 1.507454355E+00 4.945273572E+00 7.070417328E+00
17 2.517953043E+00 4.945273572E+00 7.070417328E+00
18 3.528451731E+00 4.945273572E+00 7.070417328E+00
19 4.538950418E+00 4.945273572E+00 7.070417328E+00
20 4.969556676E-01 4.945273572E+00 8.070417328E+00
21 1.507454355E+00 4.945273572E+00 8.070417328E+00
22 2.517953043E+00 4.945273572E+00 8.070417328E+00
23 3.528451731E+00 4.945273572E+00 8.070417328E+00
24 4.538950418E+00 4.945273572E+00 8.070417328E+00
25 7.163622334E+00 4.945273572E+00 7.070417328E+00
26 6.356535720E+00 4.945273572E+00 7.070417328E+00
27 7.163622334E+00 4.945273572E+00 8.070417328E+00
28 6.356535720E+00 4.945273572E+00 8.070417328E+00
29 -5.135430201E-01 4.937399556E+00 8.070417328E+00
30 -5.135430201E-01 4.937399556E+00 7.070417328E+00
31 -1.320629634E+00 4.937399556E+00 7.070417328E+00
32 -1.320629634E+00 4.937399556E+00 8.070417328E+00
33 4.538950418E+00 4.937399556E+00 7.070417328E+00
34 3.528451731E+00 4.937399556E+00 7.070417328E+00
35 2.517953043E+00 4.937399556E+00 7.070417328E+00
36 1.507454355E+00 4.937399556E+00 7.070417328E+00
37 4.969556676E-01 4.937399556E+00 7.070417328E+00
38 4.538950418E+00 4.937399556E+00 8.070417328E+00
39 3.528451731E+00 4.937399556E+00 8.070417328E+00
40 2.517953043E+00 4.937399556E+00 8.070417328E+00
41 1.507454355E+00 4.937399556E+00 8.070417328E+00
42 4.969556676E-01 4.937399556E+00 8.070417328E+00
43 6.356535720E+00 4.937399556E+00 7.070417328E+00
44 6.356535720E+00 4.937399556E+00 8.070417328E+00
45 -2.127716248E+00 4.950273572E+00 7.070417328E+00
46 -2.127716248E+00 4.950273572E+00 8.070417328E+00
47 -5.135430201E-01 4.950273572E+00 7.070417328E+00
48 -5.135430201E-01 4.950273572E+00 8.070417328E+00
49 -1.320629634E+00 4.950273572E+00 7.070417328E+00
50 -1.320629634E+00 4.950273572E+00 8.070417328E+00
51 5.549449106E+00 4.950273572E+00 7.070417328E+00
52 5.549449106E+00 4.950273572E+00 8.070417328E+00
53 7.163622334E+00 4.950273572E+00 7.070417328E+00
54 7.163622334E+00 4.950273572E+00 8.070417328E+00
55 6.356535720E+00 4.950273572E+00 7.070417328E+00
56 6.356535720E+00 4.950273572E+00 8.070417328E+00
57 -2.127716248E+00 4.932399556E+00 7.070417328E+00
58 -2.127716248E+00 4.932399556E+00 8.070417328E+00
59 -5.135430201E-01 4.932399556E+00 8.070417328E+00
60 -5.135430201E-01 4.932399556E+00 7.070417328E+00
61 -1.320629634E+00 4.932399556E+00 8.070417328E+00
62 -1.320629634E+00 4.932399556E+00 7.070417328E+00
63 5.549449106E+00 4.932399556E+00 7.070417328E+00
64 5.549449106E+00 4.932399556E+00 8.070417328E+00
65 7.163622334E+00 4.932399556E+00 7.070417328E+00
66 7.163622334E+00 4.932399556E+00 8.070417328E+00
67 6.356535720E+00 4.932399556E+00 7.070417328E+00
68 6.356535720E+00 4.932399556E+00 8.070417328E+00
-1
/wb,elem,start ! set before creation of elements
/com,*********** Elements for Body 1 "ribbon_236mm" ***********
et,1,190
eblock,19,solid,,10
(19i9)
1 1 1 1 0 0 0 0 8 0 1 9 10 12 11 30 29 32 31
1 1 1 1 0 0 0 0 8 0 2 5 6 32 31 7 8 12 11
1 1 1 1 0 0 0 0 8 0 3 9 15 20 10 30 37 42 29
1 1 1 1 0 0 0 0 8 0 4 15 16 21 20 37 36 41 42
1 1 1 1 0 0 0 0 8 0 5 16 17 22 21 36 35 40 41
1 1 1 1 0 0 0 0 8 0 6 17 18 23 22 35 34 39 40
1 1 1 1 0 0 0 0 8 0 7 18 19 24 23 34 33 38 39
1 1 1 1 0 0 0 0 8 0 8 1 33 38 2 13 19 24 14
1 1 1 1 0 0 0 0 8 0 9 3 43 44 4 25 26 28 27
1 1 1 1 0 0 0 0 8 0 10 1 2 44 43 13 14 28 26
-1
!Material Id = {225E04D9-2D24-466F-A514-34B26477580B}
sectype,1,shell
secdata,1.0 ! dummy shell thickness so SOLH190 can use a section to handle multiple integration points
/com,*********** Elements for Body 2 "Pzt_41mm" ***********
et,2,190
eblock,19,solid,,2
(19i9)
2 2 1 2 0 0 0 0 8 0 11 9 11 12 10 47 49 50 48
2 2 1 2 0 0 0 0 8 0 12 7 8 12 11 45 46 50 49
-1
!Material Id = {7AB436A5-C4E3-4C1A-A69D-527902346398}
sectype,2,shell
secdata,1.0 ! dummy shell thickness so SOLH190 can use a section to handle multiple integration points
/com,*********** Elements for Body 3 "Pzt_41mm" ***********
et,3,190
eblock,19,solid,,2
(19i9)
3 3 1 3 0 0 0 0 8 0 13 25 26 28 27 53 55 56 54
3 3 1 3 0 0 0 0 8 0 14 13 14 28 26 51 52 56 55
-1
!Material Id = {3471B5A4-22E5-4BDA-8218-9BD93B5ED02D}
sectype,3,shell
secdata,1.0 ! dummy shell thickness so SOLH190 can use a section to handle multiple integration points
/com,*********** Elements for Body 4 "Pzt_41mm" ***********
et,4,190
eblock,19,solid,,2
(19i9)
4 4 1 4 0 0 0 0 8 0 15 29 32 31 30 59 61 62 60
4 4 1 4 0 0 0 0 8 0 16 5 31 32 6 57 62 61 58
-1
!Material Id = {0E822BB1-D61B-41AD-9530-552401CF2871}
sectype,4,shell
secdata,1.0 ! dummy shell thickness so SOLH190 can use a section to handle multiple integration points
/com,*********** Elements for Body 5 "Pzt_41mm" ***********
et,5,190
eblock,19,solid,,2
(19i9)
5 5 1 5 0 0 0 0 8 0 17 3 4 44 43 65 66 68 67
5 5 1 5 0 0 0 0 8 0 18 1 43 44 2 63 67 68 64
-1
!Material Id = {EA4BD7A3-7A94-4D77-A3B8-A09F14DDCEF0}
sectype,5,shell
secdata,1.0 ! dummy shell thickness so SOLH190 can use a section to handle multiple integration points
/wb,elem,end ! done creating elements
/com,*********** Send User Defined Coordinate System(s) ***********
local,12,0,2.51795304289541,4.94527357152971,7.57041732848858,0.,0.,0.
csys,0
toffst,459.67, ! Temperature offset from absolute zero
/com,*********** Set Reference Temperature ***********
tref,71.6
/wb,mat,start ! starting to send materials
/com,*********** Send Materials ***********
MP,DENS,1,0.000205859603100009, ! slinch in^-3
MP,EX,1,362594.344285295, ! slinch s^-2 in^-1
MP,NUXY,1,0.25,
MP,DENS,2,0.000729865865536395, ! slinch in^-3
MP,EX,2,9717528.4268459, ! slinch s^-2 in^-1
MP,NUXY,2,0.483613817537644,
MP,DENS,3,0.000729865865536395, ! slinch in^-3
MP,EX,3,9717528.4268459, ! slinch s^-2 in^-1
MP,NUXY,3,0.483613817537644,
MP,DENS,4,0.000729865865536395, ! slinch in^-3
MP,EX,4,9717528.4268459, ! slinch s^-2 in^-1
MP,NUXY,4,0.483613817537644,
MP,DENS,5,0.000729865865536395, ! slinch in^-3
MP,EX,5,9717528.4268459, ! slinch s^-2 in^-1
MP,NUXY,5,0.483613817537644,
/wb,mat,end ! done sending materials
!************************* Model Summary ********************
!ribbon_236mm, Punnag powerfilm module, matid, 1
!Pzt_41mm, Mide QP16N - isotropic, matid, 2
!Pzt_41mm, Mide QP16N - isotropic, matid, 3
!Pzt_41mm, Mide QP16N - isotropic, matid, 4
!Pzt_41mm, Mide QP16N - isotropic, matid, 5
!************************* End Model Summary ********************
! get the diagonal of the bounding box. Needed later for other things
*get,_xmin,node,,mnloc,x
*get,_ymin,node,,mnloc,y
*get,_zmin,node,,mnloc,z
*get,_xmax,node,,mxloc,x
*get,_ymax,node,,mxloc,y
*get,_zmax,node,,mxloc,z
_ASMDIAG=(_xmax-_xmin)*(_xmax-_xmin)+(_ymax-_ymin)*(_ymax-_ymin)+(_zmax-_zmin)*(_zmax-_zmin)
_ASMDIAG=SQRT(_ASMDIAG)
/wb,contact,start ! starting to send contact
/wb,contact,end ! done creating contacts
/golist
/wb,load,start ! starting to send loads
/com,*********** Fixed Supports ***********
CMBLOCK,_FIXEDSU,NODE, 16
(8i10)
3 4 5 6 7 8 25 27
45 46 53 54 57 58 65 66
cmsel,s,_FIXEDSU
d,all,all
nsel,all
/gst,on,on
fini
*get,_numnode,node,0,count
*get,_numelem,elem,0,count
*get, _MAXELEMNUM, elem, 0, NUM, MAX
*get, _MAXNODENUM, node, 0, NUM, MAX
*get, _MAXELEMTYPE, etyp, 0, NUM, MAX
*get, _MAXREALCONST, real, 0, NUM, MAX
/go
/wb,load,end ! done creating loads
/com,--- Number of total nodes = %_numnode%
/com,--- Number of contact elements = 0
/com,--- Number of spring elements = 0
/com,--- Number of bearing elements = 0
/com,--- Number of solid elements = 18
/com,--- Number of condensed parts = 0
/com,--- Number of total elements = %_numelem%
*get,_wallbsol,active,,time,wall
/com,****************************************************************************
/com,************************* SOLUTION ********************************
/com,****************************************************************************
/solu
antype,4 ! transient analysis
nlgeom,on ! Turn on Large Deformation Effects
kbc,1 ! stepped BC's
eqsl,sparse,,,,,1
cntr,print,1 ! print out contact info and also make no initial contact an error
dmpoption,emat,no ! Don't combine emat file for DANSYS
dmpoption,esav,no ! Don't combine esav file for DANSYS
trnopt,full,,,,,hht ! HHT time integration method
alphad,5.e-003 ! Alpha damping
betad,1.2e-002 ! Beta damping, frequency dependent
tintp,0.1 ! Numerical Damping
nldiag,cont,iter ! print out contact info each equilibrium iteration
rescontrol,define,last,last,,dele ! Program Controlled
/com,****************************************************
/com,******************* SOLVE FOR LS 1 OF 1 ****************
/com,*********** Create Acceleration ***********
!
! ANSYS Function Representation
!
*DIM,_acelx,TABLE,6,16,2,,,,0
!
! Begin of equation: time (in/s²
_acelx(0,0,1)= 0, -999
_acelx(2,0,1)= 0.0
_acelx(3,0,1)= 0.0
_acelx(4,0,1)= 0.0
_acelx(5,0,1)= 0.0
_acelx(6,0,1)= 0.0
_acelx(0,1,1)= 1.0, -1, 0, 3.93700787401575E-02, 0, 0, 1
_acelx(0,2,1)= 0.0, -2, 0, 1, 1, 3, -1
_acelx(0,3,1)= 0, 99, 0, 1, -2, 0, 0
_acelx(0,4,1)= 0.0,
_acelx(0,5,1)= 0.0,
_acelx(0,6,1)= 0.0,
_acelx(0,7,1)= 0.0,
_acelx(0,8,1)= 0.0,
_acelx(0,9,1)= 0.0,
_acelx(0,10,1)= 0.0,
_acelx(0,11,1)= 0.0,
_acelx(0,12,1)= 0.0,
_acelx(0,13,1)= 0.0,
_acelx(0,14,1)= 0.0,
_acelx(0,15,1)= 0.0,
_acelx(0,16,1)= 0.0,
! End of equation: time (in/s²
!
! Begin of equation: (-0.3*9800*sin(2*3.142*9.44*time))*0.0 (in/s²
_acelx(0,0,2)= -999, -999
_acelx(2,0,2)= 0.0
_acelx(3,0,2)= 0.0
_acelx(4,0,2)= 0.0
_acelx(5,0,2)= 0.0
_acelx(6,0,2)= 0.0
_acelx(0,1,2)= 1.0, -1, 0, -0.3, 0, 0, 0
_acelx(0,2,2)= 0.0, -2, 0, 9800, 0, 0, -1
_acelx(0,3,2)= 0, -3, 0, 1, -1, 3, -2
_acelx(0,4,2)= 0.0, -1, 0, 2, 0, 0, 0
_acelx(0,5,2)= 0.0, -2, 0, 3.142, 0, 0, -1
_acelx(0,6,2)= 0.0, -4, 0, 1, -1, 3, -2
_acelx(0,7,2)= 0.0, -1, 0, 9.44, 0, 0, -4
_acelx(0,8,2)= 0.0, -2, 0, 1, -4, 3, -1
_acelx(0,9,2)= 0.0, -1, 0, 1, -2, 3, 1
_acelx(0,10,2)= 0.0, -1, 9, 1, -1, 0, 0
_acelx(0,11,2)= 0.0, -2, 0, 1, -3, 3, -1
_acelx(0,12,2)= 0.0, -1, 0, 0, 0, 0, -2
_acelx(0,13,2)= 0.0, -3, 0, 1, -2, 3, -1
_acelx(0,14,2)= 0.0, -1, 0, 3.93700787401575E-02, 0, 0, -3
_acelx(0,15,2)= 0.0, -2, 0, 1, -3, 3, -1
_acelx(0,16,2)= 0.0, 99, 0, 1, -2, 0, 0
! End of equation: (-0.3*9800*sin(2*3.142*9.44*time))*0.0 (in/s²
!
! ANSYS Function Representation
!
*DIM,_acely,TABLE,6,16,2,,,,0
!
! Begin of equation: time (in/s²
_acely(0,0,1)= 0, -999
_acely(2,0,1)= 0.0
_acely(3,0,1)= 0.0
_acely(4,0,1)= 0.0
_acely(5,0,1)= 0.0
_acely(6,0,1)= 0.0
_acely(0,1,1)= 1.0, -1, 0, 3.93700787401575E-02, 0, 0, 1
_acely(0,2,1)= 0.0, -2, 0, 1, 1, 3, -1
_acely(0,3,1)= 0, 99, 0, 1, -2, 0, 0
_acely(0,4,1)= 0.0,
_acely(0,5,1)= 0.0,
_acely(0,6,1)= 0.0,
_acely(0,7,1)= 0.0,
_acely(0,8,1)= 0.0,
_acely(0,9,1)= 0.0,
_acely(0,10,1)= 0.0,
_acely(0,11,1)= 0.0,
_acely(0,12,1)= 0.0,
_acely(0,13,1)= 0.0,
_acely(0,14,1)= 0.0,
_acely(0,15,1)= 0.0,
_acely(0,16,1)= 0.0,
! End of equation: time (in/s²
!
! Begin of equation: (-0.3*9800*sin(2*3.142*9.44*time))*1 (in/s²
_acely(0,0,2)= -999, -999
_acely(2,0,2)= 0.0
_acely(3,0,2)= 0.0
_acely(4,0,2)= 0.0
_acely(5,0,2)= 0.0
_acely(6,0,2)= 0.0
_acely(0,1,2)= 1.0, -1, 0, -0.3, 0, 0, 0
_acely(0,2,2)= 0.0, -2, 0, 9800, 0, 0, -1
_acely(0,3,2)= 0, -3, 0, 1, -1, 3, -2
_acely(0,4,2)= 0.0, -1, 0, 2, 0, 0, 0
_acely(0,5,2)= 0.0, -2, 0, 3.142, 0, 0, -1
_acely(0,6,2)= 0.0, -4, 0, 1, -1, 3, -2
_acely(0,7,2)= 0.0, -1, 0, 9.44, 0, 0, -4
_acely(0,8,2)= 0.0, -2, 0, 1, -4, 3, -1
_acely(0,9,2)= 0.0, -1, 0, 1, -2, 3, 1
_acely(0,10,2)= 0.0, -1, 9, 1, -1, 0, 0
_acely(0,11,2)= 0.0, -2, 0, 1, -3, 3, -1
_acely(0,12,2)= 0.0, -1, 0, 1, 0, 0, -2
_acely(0,13,2)= 0.0, -3, 0, 1, -2, 3, -1
_acely(0,14,2)= 0.0, -1, 0, 3.93700787401575E-02, 0, 0, -3
_acely(0,15,2)= 0.0, -2, 0, 1, -3, 3, -1
_acely(0,16,2)= 0.0, 99, 0, 1, -2, 0, 0
! End of equation: (-0.3*9800*sin(2*3.142*9.44*time))*1 (in/s²
!
! ANSYS Function Representation
!
*DIM,_acelz,TABLE,6,16,2,,,,0
!
! Begin of equation: time (in/s²
_acelz(0,0,1)= 0, -999
_acelz(2,0,1)= 0.0
_acelz(3,0,1)= 0.0
_acelz(4,0,1)= 0.0
_acelz(5,0,1)= 0.0
_acelz(6,0,1)= 0.0
_acelz(0,1,1)= 1.0, -1, 0, 3.93700787401575E-02, 0, 0, 1
_acelz(0,2,1)= 0.0, -2, 0, 1, 1, 3, -1
_acelz(0,3,1)= 0, 99, 0, 1, -2, 0, 0
_acelz(0,4,1)= 0.0,
_acelz(0,5,1)= 0.0,
_acelz(0,6,1)= 0.0,
_acelz(0,7,1)= 0.0,
_acelz(0,8,1)= 0.0,
_acelz(0,9,1)= 0.0,
_acelz(0,10,1)= 0.0,
_acelz(0,11,1)= 0.0,
_acelz(0,12,1)= 0.0,
_acelz(0,13,1)= 0.0,
_acelz(0,14,1)= 0.0,
_acelz(0,15,1)= 0.0,
_acelz(0,16,1)= 0.0,
! End of equation: time (in/s²
!
! Begin of equation: (-0.3*9800*sin(2*3.142*9.44*time))*0.0 (in/s²
_acelz(0,0,2)= -999, -999
_acelz(2,0,2)= 0.0
_acelz(3,0,2)= 0.0
_acelz(4,0,2)= 0.0
_acelz(5,0,2)= 0.0
_acelz(6,0,2)= 0.0
_acelz(0,1,2)= 1.0, -1, 0, -0.3, 0, 0, 0
_acelz(0,2,2)= 0.0, -2, 0, 9800, 0, 0, -1
_acelz(0,3,2)= 0, -3, 0, 1, -1, 3, -2
_acelz(0,4,2)= 0.0, -1, 0, 2, 0, 0, 0
_acelz(0,5,2)= 0.0, -2, 0, 3.142, 0, 0, -1
_acelz(0,6,2)= 0.0, -4, 0, 1, -1, 3, -2
_acelz(0,7,2)= 0.0, -1, 0, 9.44, 0, 0, -4
_acelz(0,8,2)= 0.0, -2, 0, 1, -4, 3, -1
_acelz(0,9,2)= 0.0, -1, 0, 1, -2, 3, 1
_acelz(0,10,2)= 0.0, -1, 9, 1, -1, 0, 0
_acelz(0,11,2)= 0.0, -2, 0, 1, -3, 3, -1
_acelz(0,12,2)= 0.0, -1, 0, 0, 0, 0, -2
_acelz(0,13,2)= 0.0, -3, 0, 1, -2, 3, -1
_acelz(0,14,2)= 0.0, -1, 0, 3.93700787401575E-02, 0, 0, -3
_acelz(0,15,2)= 0.0, -2, 0, 1, -3, 3, -1
_acelz(0,16,2)= 0.0, 99, 0, 1, -2, 0, 0
! End of equation: (-0.3*9800*sin(2*3.142*9.44*time))*0.0 (in/s²
acel,%_acelx%,%_acely%,%_acelz%
/nopr
/gopr
autots,on ! User turned on automatic time stepping
deltim,0.001,0.0001,0.005,OFF
time,5.
timint,on ! Turn on time integration effects
outres,erase
outres,all,none
outres,nsol,all,
outres,rsol,all
outres,strs,all,
outres,epel,all,
outres,eppl,all,
outres,v,all,
outres,a,all,
stabilize,off ! Stabilization turned OFF by user
! *********** WB SOLVE COMMAND ***********
! check interactive state
*get,ANSINTER_,active,,int
*if,ANSINTER_,ne,0,then
/eof
*endif
solve
/com *************** Write FE CONNECTORS *********
CEWRITE,file,ce,,INTE
/com,****************************************************
/com,*************** FINISHED SOLVE FOR LS 1 *************
*get,_wallasol,active,,time,wall
/nopr
*get,_numnode,node,0,count
*get,_numelem,elem,0,count
*get, _MAXELEMNUM, elem, 0, NUM, MAX
*get, _MAXNODENUM, node, 0, NUM, MAX,,,INTERNAL
*get, _MAXELEMTYPE, etyp, 0, NUM, MAX
*get, _MAXREALCONST, real, 0, NUM, MAX
/gopr
/post1
xmlo,ENCODING,ISO-8859-1
xmlo,parm
/xml,parm,xml
fini
/gopr
*get,_walldone,active,,time,wall
_preptime=(_wallbsol-_wallstrt)*3600
_solvtime=(_wallasol-_wallbsol)*3600
_posttime=(_walldone-_wallasol)*3600
_totaltim=(_walldone-_wallstrt)*3600
/wb,file,end ! done with WB generated input
Regards,
Peter
-
peteroznewman I have found the solution to write the command snippet that would print the table to file. However, it does not print the probe data but it can print a "named selection" nodal point's displacement vs time data. Which also works for my case
Then in the APDL command snippet, the code is this:
!*********************************APDL code snippet*****************************************
set,last
*get, nsets,active,0,set,nset
*dim, data_store,,nsets,2
*do,i,1,nsets
set,next
*get,t,active,,set,time
cmsel,s,Probe_pt
*get,node_id,node,0,num,max
*get,displ,node,node_id,U,sum
data_store(i,1) = t
data_store(i,2) = displ
*enddo
*cfopen,try,txt !filename written is try.txt which is a 2 column table of time and displacements
*vwrite,data_store(1,1), data_store(1,2)
%g %g
*cfclos
!*********************************END of APDL code snippet*****************************************
This works and I have verified this.
Now my next question is how do I run "input_.dat" file from MATLAB? Is it possible?
-
-
-
-
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
-
Rob
-
Guilin Sun
-
peteroznewman
-
DrAmine
-
javat33489
You are navigating away from the AIS Discovery experience