How to run scripts in APDL
Before we begin the actual scripting, let's do a quick tutorial on some of the methods of running scripts in APDL.
| Expand | ||
|---|---|---|
| ||
Scrips in APDL are usually executed by the use of one of two methods. The first method is to write (or copy & paste) your code directly into the command window available in APDL.
The other method is to read in an input file (txt file) containing your script. To do this, go to File → Read Input From, select the correct file form the menu and click OK.
When locating the correct file, you will often notice that APDL by default opens the wrong directory (e.g. C:USERS when you actually want ../Marine Konstruksjoner/Exercise 7). To fix this, we need to open APDL with our chosen working directory. We may do so by first opening the ANSYS Mechanical APDL Product Launcher and then choose the correct working directory before clicking Run.
|
Introduction to APDL commands
Although many APDL commands are similar to what we are familiar with from other programming languages, very few have the exact same syntax. This means that to fully understand your code, and to further improve it, you will have to read the APDL commands documentation.
| Info |
|---|
The easiest way to locate the correct documentation is to open Mechanical APDL and click Help → Help Topics. Since we will focus on the scripting part of APDL, the Command reference documentation is the most relevant to us.
|
As a first example, we would like to obtain the stresses in the node located in the point (L/2, H/2) and write them into our file answers.txt, given the plate below.
The following script includes some simple comments for most commands, but to truly understand the code, we highly recommend you to search them up in the Command Reference as well.
| Code Block | ||||||
|---|---|---|---|---|---|---|
| ||||||
! Author: Chana Sinsabvarodom ! Edited by: Jon Arnt Kårstad !======================== ! Initial programming setup FINISH /CLEAR ! Clear all /PREP7 ! Enter preprocessor /UNITS,SI ! Use SI units !======================== ! Defining the variables !======================== L=0.6 ! Length [m] H=0.2 ! Height [m] t=0.005 ! Thickness [m] Diameter = H*0.3 ! Diameter of hole [m] Length2hole = L*0.5 ! Length to hole [m] P=-50e6*t ! Load, we will use as a pressure load [Pa] (positive - compression, negative - tension) mesh_size=0.01 ! Mesh size ! Making the plate K,,0,-H/2,0 ! Lower left node K,,L,-H/2,0 ! Lower right node K,,L,H/2,0 ! Upper right node K,,0,H/2,0 ! Upper left node A,1,2,3,4 ! Making an area from our nodes (notice the order) CYL4,Length2hole,0,Diameter/2, ! Make cylinder ASBA,1,2 ! Remove area 2 (cylinder) from area 1 (plate) !======================== ! Defining the material data (here aluminium) !======================== MPTEMP,1,0 MPDATA,EX,1,,0.69e11 ! Young's modulus [Pa] MPDATA,PRXY,1,,0.3 ! Poisson's ratio [-] MPDATA,DENS,1,,2700 ! Density [kg/m^3] !======================== ! Define local element type !======================== ET,1,SHELL181 ! Shell element, both bending and membrane stresses !======================== ! Connecting area to component !======================== ASEL,S,LOC,Z,0 ! Select area at z = 0 CM,PLATE,AREA ! Group geometry into component ALLSEL,ALL ! Select all !======================== ! Assigning a thickness to the plate !======================== SECTYPE,1,SHELL,,PLATE ! Associates section type information with a section ID number. SECDATA,T,1,0,3 ! Given section data SECOFFSET,MID ! Define section offset for cross section !======================== ! Defining the mesh !======================== ESIZE,MESH_SIZE ! Element size TYPE,1 ! Set element type pointer SECNUM,1 ! Set element section attribute pointer CMSEL,S,PLATE,AREA ! Select component named plate (of type area) AMESH,PLATE ! Mesh plate /ESHAPE,1 !======================== ! Load !======================== NSEL,S,LOC,X,L ! Select all nodes at x = L SF,ALL,PRES,P ! Apply pressure load to nodes selected !======================== ! Boundary conditions (Select All X) !======================== NSEL,S,LOC,X,0 ! Select all nodes at x = 0 D,ALL,UX,0,,,,UY,UZ,ROTX,ROTY,ROTZ ! Apply boundary conditions to nodes selected ALLSEL,ALL !======================== ! Solution !======================== ! Notice that from now on we write only lower case letters ! APDL does does not differentiate between letter cases (lower or upper, 'A' or 'a') ! It therefore does not matter here, but care, it may cause trouble when working with variables /solu ! Enter solution processor solve ! Start a solution /post1 ! Enters database results postprocessor /gline,,-1 ! Don't show element lines (0 - solid lines, 1 - dashed lines) plnsol,s,eqv ! Display results as continous element contours !======================== ! Write results to text file !======================== ! When writing a file, it is often clever to specify where you want to store the file first /cwd,'C:\....WRITE YOUR OWN PATH HERE' ! Changing working directory *cfopen,answers.txt,,,append ! Open file, append (means add to end of file) !======================== ! Example task 1 !======================== *vwrite,'Meshsize','XX','YY','XY','Von Mises' ! Write text (A13,A13,A13,A13,A13,A13) ! A = string ! Above we need to specify how much space we want to give the text. The text is then right-aligned ! x = L/2 and y = H/2 -> mid top node s1=node(L/2, H/2, 0) ! Select node *GET,normal_stress_x,node,s1,s,x ! Results Stress X (sigma_x) *GET,normal_stress_y,node,s1,s,y ! Results Stress Y (sigma_y) *GET,shear_stress,node,s1,s,xy ! Results Stress XY (tau_xy) *GET,stress_von_mises,node,s1,s,eqv ! Results Stress Von Mises *vwrite,mesh_size,normal_stress_x,normal_stress_y,shear_stress,stress_von_mises (E13.3,E13.3,E13.3,E13.3,E13.3) ! E = Exponential form *cfclos ! Close file |
The following result file will then be created.
| Code Block | ||||||
|---|---|---|---|---|---|---|
| ||||||
Meshsize XX YY XY Von Mise
0.100E-01 0.481E+08 0.500E+06 -0.686E+05 0.479E+08 |
Loops and statements in APDL?
When doing FEM-analyses, we are often looking to locate e.g. how large our load is before buckling or how small the mesh size has to be before the results converges. If we were to do these tasks manually, it would take forever, and it is for that reason APDL has included loops and statements.
As an example, let's do the analysis presented in the previous section, but for mesh size = 0.10 to mesh size = 0.01 with a step size of 0.01.
| Code Block | ||||||
|---|---|---|---|---|---|---|
| ||||||
!======================== ! Initial programming setup before entering the loop !======================== FINISH /CLEAR !======================== ! Defining the variables !======================== L=0.6 ! Length [m] H=0.2 ! Height [m] t=0.005 ! Thickness [m] Diameter = H*0.3 ! Diameter of hole [m] Length2hole = L*0.5 ! Length to hole [m] P=-50e6*t ! Load, we will use as a pressure load [Pa] (positive - compression, negative - tension) mesh_size = 0.10 ! Initial mesh size ! We only want to write this section on the very top of our file /cwd,'C:\....WRITE YOUR OWN PATH HERE' ! Changing working directory *cfopen,answers.txt,,,append ! Open file, append (means add to end of file) *vwrite,'Meshsize','XX','YY','XY','Von Mises' ! Write text (A13,A13,A13,A13,A13,A13) ! A = string !======================== ! Start of loop !======================== condition = 1 ! We want an infinite loop *DOWHILE, condition ! Regular while loop with condition *IF,mesh_size,EQ,0.01,EXIT ! If mesh_size == 0.01, exit loop !======================== ! Initial programming setup !======================== ! To clear area, mesh etc, but not all variables, we first write all variables to a separate file ! The reason for this is mainly because we want to keep the mesh_size and our condition PARSAV,,param FINISH /CLEAR ! After clear, we read in the variables we had previously. PARRES,,param /PREP7 /UNITS, SI !======================== ! Making plate !======================== K,,0,-H/2,0 ! Lower left node K,,L,-H/2,0 ! Lower right node K,,L,H/2,0 ! Upper right node K,,0,H/2,0 ! Upper left node A,1,2,3,4 ! Making an area from our nodes (notice the order) CYL4,Length2hole,0,Diameter/2, ! Make cylinder ASBA,1,2 ! Remove area 2 (cylinder) from area 1 (plate) !======================== ! Defining the material data (here aluminium) !======================== MPTEMP,1,0 MPDATA,EX,1,,0.69e11 ! Young's modulus [Pa] MPDATA,PRXY,1,,0.3 ! Poisson's ratio [-] MPDATA,DENS,1,,2700 ! Density [kg/m^3] !======================== ! Define local element type !======================== ET,1,SHELL181 ! Shell element, both bending and membrane stresses !======================== ! Connecting area to component !======================== ASEL,S,LOC,Z,0 ! Select area at z = 0 CM,PLATE,AREA ! Group geometry into component ALLSEL,ALL ! Select all !======================== ! Assigning a thickness to the plate !======================== SECTYPE,1,SHELL,,PLATE ! Associates section type information with a section ID number. SECDATA,T,1,0,3 ! Given section data SECOFFSET,MID ! Define section offset for cross section !======================== ! Defining the mesh !======================== ESIZE,MESH_SIZE ! Element size TYPE,1 ! Set element type pointer SECNUM,1 ! Set element section attribute pointer CMSEL,S,PLATE,AREA ! Select component named plate (of type area) AMESH,PLATE ! Mesh plate /ESHAPE,1 !======================== ! Load !======================== NSEL,S,LOC,X,L ! Select all nodes at x = L SF,ALL,PRES,P ! Apply pressure load to nodes selected !======================== ! Boundary conditions (Select All X) !======================== NSEL,S,LOC,X,0 ! Select all nodes at x = 0 D,ALL,UX,0,,,,UY,UZ,ROTX,ROTY,ROTZ ! Apply boundary conditions to nodes selected ALLSEL,ALL !======================== ! Solution !======================== /solu ! Enter solution processor solve ! Start a solution /post1 ! Enters database results postprocessor /gline,,-1 ! Don't show element lines (0 - solid lines, 1 - dashed lines) plnsol,s,eqv ! Display results as continous element contours !======================== ! Write results to text file !======================== ! When writing a file, it is often clever to specify where you want to store the file first /cwd,'C:\....WRITE YOUR OWN PATH HERE' ! Changing working directory *cfopen,answers.txt,,,append ! Open file, append (means add to end of file) !======================== ! Example task 2 !======================== ! x = L/2 and y = H/2 -> mid top node s1=node(L/2, H/2, 0) ! Select node *GET,normal_stress_x,node,s1,s,x ! Results Stress X (sigma_x) *GET,normal_stress_y,node,s1,s,y ! Results Stress Y (sigma_y) *GET,shear_stress,node,s1,s,xy ! Results Stress XY (tau_xy) *GET,stress_von_mises,node,s1,s,eqv ! Results Stress Von Mises *vwrite,mesh_size,normal_stress_x,normal_stress_y,shear_stress,stress_von_mises (E13.3,E13.3,E13.3,E13.3,E13.3) ! E = Exponential form *cfclos ! Close file mesh_size = mesh_size - 0.01 ! Decrease mesh size *ENDDO ! End of while loop |
The following result file will then be created.
| Code Block | ||||||
|---|---|---|---|---|---|---|
| ||||||
Meshsize XX YY XY Von Mise
0.100E+00 0.592E+08 0.203E+07 -0.428E+05 0.582E+08
0.900E-01 0.552E+08 -0.294E+06 0.300E+06 0.553E+08
0.800E-01 0.543E+08 -0.671E+06 0.106E+07 0.546E+08
0.700E-01 0.577E+08 -0.360E+07 0.222E+07 0.597E+08
0.600E-01 0.618E+08 0.473E+06 0.276E+07 0.617E+08
0.500E-01 0.605E+08 0.668E+06 -0.158E+07 0.602E+08
0.400E-01 0.551E+08 0.169E+07 0.149E+07 0.543E+08
0.300E-01 0.528E+08 0.988E+06 0.199E+05 0.523E+08
0.200E-01 0.513E+08 0.974E+06 0.538E+05 0.508E+08
|
File output format
If you're new to APDL, the output formatting may feel a bit weird at first. However, the format descriptors may be written in either FORTRAN or C format, where as we will cover both. Before we begin, I want to remind you that there are a lot of other good documentation on these format descriptors online if you should not find what you are looking for here. Such pages may be this FORTRAN guide by the Michigan Tecnological University or this C guide by cplusplus.com. In addition, ANSYS has included some additional information in their command reference on *vwrite.
Let's first start with the FORTRAN format, which is also what has been used in the previous example scripts.
| Expand | |||||||||||||||||||||||||||||||||||||||||||
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| |||||||||||||||||||||||||||||||||||||||||||
The following table includes most of editor descriptors used in FORTRAN. To present it as simple as possible, the following convention of symbols are used:
Although APDL uses FORTRAN formatting, there are some limitations. You may have already spotted one in the previous examples, where the "s" in "Von Mises" has been absent from the file output. The following information are obtained from the APDL command reference. "Alphanumeric strings are limited to a maximum of 8 characters for any field (A8) using the FORTRAN format. Use the “C” format for string arrays larger than 8 characters. Integer (I) and list-directed (*) descriptors may not be used. You can include text in the format as a quoted string. The parentheses must be included in the format and the format must not exceed 80 characters (including parentheses). The output line length is limited to 128 characters." The script "Script_output.txt" is used to display some examples using the FORTRAN formatting.
The file "answer.txt" is the resulting file when running the script above.
| |||||||||||||||||||||||||||||||||||||||||||
The other possibility is to use the C format.
| Expand | ||||||||||||||||||||||||||||||||||||||||||||||||
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| ||||||||||||||||||||||||||||||||||||||||||||||||
As with the FORTRAN format, we will start out with a table presenting some of the editor descriptors used in C. To present it as simple as possible, the following convention of symbols are used:
To distinguish between using the C or FORTRAN format, ADPL has provided the following information. "The “C” format descriptors are used if the first character of the format descriptor line is not a left parenthesis. “C” format descriptors are up to 80 characters long, consisting of text strings and predefined "data descriptors" between the strings where numeric or alphanumeric character data will be inserted." The script "Script_output.txt" is used to display some examples using the FORTRAN formatting.
The file "answer.txt" is the resulting file when running the script above.
| ||||||||||||||||||||||||||||||||||||||||||||||||
| BibTeX Display Table |
|---|