liminfoANSYS Reference
Free reference guide: ANSYS Reference
About ANSYS Reference
The ANSYS APDL Reference is a practical quick-lookup guide for ANSYS Mechanical APDL (ANSYS Parametric Design Language) commands and concepts. It covers the most commonly used structural element types including SOLID186 (20-node hex), SOLID187 (10-node tet), SHELL181 (4-node shell with section data), BEAM188 (2-node beam with cross-section), and PLANE182 (2D solid for plane stress/strain analysis).
The material and loading sections provide ready-to-use syntax for defining elastic properties (MP,EX for Young's modulus, MP,PRXY for Poisson's ratio), density, plasticity models (TB,BISO for bilinear isotropic, TB,MISO for multilinear isotropic hardening), and hyperelastic models (Mooney-Rivlin). Boundary conditions include nodal forces (F command), displacement constraints (D command), surface pressures (SFA), gravitational acceleration (ACEL), and thermal body loads (BF,TEMP).
Solver and post-processing entries cover static analysis with geometric nonlinearity (NLGEOM), modal analysis (MODOPT,LANB), transient time-history analysis (DELTIM, TRNOPT), buckling analysis (BUCOPT), and the general post-processor (/POST1) for contour plots of von Mises stress (PLNSOL,S,EQV) and displacement results. APDL scripting commands (*DO loops, *IF conditionals, *GET for result extraction) are included for automation workflows.
Key Features
- 3D solid elements: SOLID186 (20-node, reduced/full integration) and SOLID187 (10-node tetrahedral for free meshing)
- Shell and beam elements: SHELL181 with SECDATA thickness and BEAM188 with rectangular/circular cross-sections
- Material models: elastic (MP,EX/PRXY), bilinear plasticity (TB,BISO), multilinear plasticity (TB,MISO), hyperelastic Mooney-Rivlin
- Boundary conditions: nodal forces (F), displacement constraints (D,ALL), surface pressure (SFA), gravity (ACEL), thermal loads (BF,TEMP)
- Solver types: static with NLGEOM, modal (LANB, MXPAND), transient (FULL/DELTIM), and buckling (BUCOPT) analysis
- Post-processing: /POST1, von Mises contour (PLNSOL,S,EQV), displacement sum (PLNSOL,U,SUM), and nodal stress output (PRNSOL)
- APDL scripting: *DO/*ENDDO loops, *IF/*ENDIF conditionals, *GET for extracting maximum stress and displacement values
- Bilingual Korean/English with categorized browsing across Elements, Materials, Loads, Solver, Post-processing, and APDL
Frequently Asked Questions
When should I use SOLID186 vs SOLID187?
SOLID186 is a 20-node hexahedral element best for mapped (structured) meshes with superior accuracy and efficiency. SOLID187 is a 10-node tetrahedral element suited for free meshing of complex geometries where hex meshing is impractical. Both support large deformation, plasticity, and reduced/full integration. Use SOLID186 when geometry allows mapped meshing; use SOLID187 for automatic free-meshing of irregular shapes.
How do I define bilinear isotropic hardening plasticity?
Use TB,BISO,matid followed by TBDATA,1,yield_stress,tangent_modulus. For example: TB,BISO,1 and TBDATA,1,250,1000 defines material 1 with 250 MPa yield stress and 1000 MPa tangent modulus. For multilinear hardening, use TB,MISO with TBPT commands to define stress-strain pairs at multiple points.
What is the difference between ANTYPE,STATIC and ANTYPE,MODAL?
ANTYPE,STATIC solves for displacements and stresses under applied loads (with optional geometric nonlinearity via NLGEOM,ON). ANTYPE,MODAL performs eigenvalue extraction to find natural frequencies and mode shapes using methods like Block Lanczos (MODOPT,LANB,n). Modal analysis does not apply external loads; it characterizes the structure's dynamic properties.
How do I apply gravity in ANSYS?
Use the ACEL command to apply acceleration. For gravity in the Y-direction with mm/s2 units: ACEL,0,9810,0. The sign depends on your coordinate system convention. Note that density (MP,DENS) must be defined for the acceleration to generate inertial loads. For tonne/mm unit system, use DENS=7.85e-9 for steel.
How do I perform a buckling analysis?
First run a static analysis to establish the pre-stress state, then switch to ANTYPE,BUCKLE with BUCOPT,LANB,n (where n is the number of buckling modes). SOLVE extracts the buckling load multipliers. The critical buckling load is the applied load multiplied by the first eigenvalue. The MXPAND command can expand mode shapes for visualization.
What does PLNSOL,S,EQV display?
PLNSOL,S,EQV displays a contour plot of von Mises equivalent stress at nodes in the general post-processor (/POST1). First use SET,LAST to read the last load step result. PRNSOL,S,COMP prints the individual stress components (SX, SY, SZ, SXY, SYZ, SXZ) at each node. PLNSOL,U,SUM shows the total displacement magnitude contour.
How do I use *GET to extract maximum stress?
After entering /POST1 and loading results with SET,LAST, use *GET,MAXS,NODE,,S,EQV,MAX to store the maximum von Mises stress in parameter MAXS. Similarly, *GET,MAXU,NODE,,U,SUM,MAX extracts the maximum displacement. These parameters can be used in *IF conditionals or written to output files for parametric studies.
How do I set up SHELL181 with thickness?
First define the element type: ET,1,SHELL181. Then create a shell section: SECTYPE,1,SHELL followed by SECDATA,thickness (e.g., SECDATA,2.0 for 2mm). Multiple layers can be defined for composites by adding additional SECDATA entries with thickness, material, and orientation angle for each layer.