.. DO NOT EDIT. .. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY. .. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE: .. "examples/00_basic/example_01_simple_structural_solve.py" .. LINE NUMBERS ARE GIVEN BELOW. .. only:: html .. note:: :class: sphx-glr-download-link-note :ref:`Go to the end ` to download the full example code. .. rst-class:: sphx-glr-example-title .. _sphx_glr_examples_00_basic_example_01_simple_structural_solve.py: .. _ref_example_01_simple_structural_solve: Static structural analysis -------------------------- Using supplied files, this example shows how to insert a static structural analysis into a new Mechanical session and execute a sequence of Python scripting commands that define and solve the analysis. The example then shows how to report deformation results. .. GENERATED FROM PYTHON SOURCE LINES 14-17 Download required files ~~~~~~~~~~~~~~~~~~~~~~~ Download the required files. Print the file path for the geometry file. .. GENERATED FROM PYTHON SOURCE LINES 17-26 .. code-block:: Python import os from ansys.mechanical.core import launch_mechanical from ansys.mechanical.core.examples import download_file geometry_path = download_file("example_01_geometry.agdb", "pymechanical", "00_basic") print(f"Downloaded the geometry file to: {geometry_path}") .. rst-class:: sphx-glr-script-out .. code-block:: none Downloaded the geometry file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_01_geometry.agdb .. GENERATED FROM PYTHON SOURCE LINES 27-32 Launch Mechanical ~~~~~~~~~~~~~~~~~ Launch a new Mechanical session in batch, setting the ``cleanup_on_exit`` argument to ``False``. To close this Mechanical session when finished, this example must call the ``mechanical.exit()`` method. .. GENERATED FROM PYTHON SOURCE LINES 32-36 .. code-block:: Python mechanical = launch_mechanical(batch=True, cleanup_on_exit=False) print(mechanical) .. rst-class:: sphx-glr-script-out .. code-block:: none Ansys Mechanical [Ansys Mechanical Enterprise] Product Version:242 Software build date: 06/03/2024 09:35:09 .. GENERATED FROM PYTHON SOURCE LINES 37-41 Initialize variable for workflow ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ Set the ``part_file_path`` variable on the server for later use. Make this variable compatible for Windows, Linux, and Docker containers. .. GENERATED FROM PYTHON SOURCE LINES 41-58 .. code-block:: Python project_directory = mechanical.project_directory print(f"project directory = {project_directory}") # Upload the file to the project directory. mechanical.upload(file_name=geometry_path, file_location_destination=project_directory) # Build the path relative to project directory. base_name = os.path.basename(geometry_path) combined_path = os.path.join(project_directory, base_name) part_file_path = combined_path.replace("\\", "\\\\") mechanical.run_python_script(f"part_file_path='{part_file_path}'") # Verify the path. result = mechanical.run_python_script("part_file_path") print(f"part_file_path on server: {result}") .. rst-class:: sphx-glr-script-out .. code-block:: none project directory = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/ Uploading example_01_geometry.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/.: 0%| | 0.00/17.0k [00:00> Ansys Product Improvement Program | | in the GUI. | | For more information about the Ansys Privacy Policy, please | | check: http://www.ansys.com/privacy | | | *------------------------------------------------------------------* 2024 R2 Point Releases and Patches installed: Ansys, Inc. License Manager 2024 R2 LS-DYNA 2024 R2 Core WB Files 2024 R2 Mechanical Products 2024 R2 ***** MAPDL COMMAND LINE ARGUMENTS ***** BATCH MODE REQUESTED (-b) = NOLIST INPUT FILE COPY MODE (-c) = COPY DISTRIBUTED MEMORY PARALLEL REQUESTED 4 PARALLEL PROCESSES REQUESTED WITH SINGLE THREAD PER PROCESS TOTAL OF 4 CORES REQUESTED INPUT FILE NAME = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/dummy.dat OUTPUT FILE NAME = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/solve.out START-UP FILE MODE = NOREAD STOP FILE MODE = NOREAD RELEASE= 2024 R2 BUILD= 24.2 UP20240603 VERSION=LINUX x64 CURRENT JOBNAME=file0 14:49:19 NOV 04, 2024 CP= 0.238 PARAMETER _DS_PROGRESS = 999.0000000 /INPUT FILE= ds.dat LINE= 0 *** NOTE *** CP = 0.346 TIME= 14:49:19 The /CONFIG,NOELDB command is not valid in a distributed memory parallel solution. Command is ignored. *GET _WALLSTRT FROM ACTI ITEM=TIME WALL VALUE= 14.8219444 TITLE= --Static Structural ACT Extensions: LSDYNA, 2024.2 5f463412-bd3e-484b-87e7-cbc0a665e474, wbex SET PARAMETER DIMENSIONS ON _WB_PROJECTSCRATCH_DIR TYPE=STRI DIMENSIONS= 248 1 1 PARAMETER _WB_PROJECTSCRATCH_DIR(1) = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/ SET PARAMETER DIMENSIONS ON _WB_SOLVERFILES_DIR TYPE=STRI DIMENSIONS= 248 1 1 PARAMETER _WB_SOLVERFILES_DIR(1) = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/ SET PARAMETER DIMENSIONS ON _WB_USERFILES_DIR TYPE=STRI DIMENSIONS= 248 1 1 PARAMETER _WB_USERFILES_DIR(1) = /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/UserFiles/ --- Data in consistent MKS units. See Solving Units in the help system for more MKS UNITS SPECIFIED FOR INTERNAL LENGTH (l) = METER (M) MASS (M) = KILOGRAM (KG) TIME (t) = SECOND (SEC) TEMPERATURE (T) = CELSIUS (C) TOFFSET = 273.0 CHARGE (Q) = COULOMB FORCE (f) = NEWTON (N) (KG-M/SEC2) HEAT = JOULE (N-M) PRESSURE = PASCAL (NEWTON/M**2) ENERGY (W) = JOULE (N-M) POWER (P) = WATT (N-M/SEC) CURRENT (i) = AMPERE (COULOMBS/SEC) CAPACITANCE (C) = FARAD INDUCTANCE (L) = HENRY MAGNETIC FLUX = WEBER RESISTANCE (R) = OHM ELECTRIC POTENTIAL = VOLT INPUT UNITS ARE ALSO SET TO MKS *** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2024 R2 24.2 *** Ansys Mechanical Enterprise 00000000 VERSION=LINUX x64 14:49:19 NOV 04, 2024 CP= 0.350 --Static Structural ***** MAPDL ANALYSIS DEFINITION (PREP7) ***** *********** Nodes for the whole assembly *********** *********** Nodes for all Remote Points *********** *** WARNING *** CP = 0.390 TIME= 14:49:19 -1 is not a recognized PREP7 command, abbreviation, or macro. This command will be ignored. *********** Elements for Body 1 'Part1' *********** *********** Elements for Body 2 'Part2' *********** *********** Elements for Body 3 'Part3' *********** *********** Elements for Body 4 'Part4' *********** *********** Send User Defined Coordinate System(s) *********** *********** Set Reference Temperature *********** *********** Send Materials *********** *********** Create Contact "Contact Region" *********** Real Constant Set For Above Contact Is 6 & 5 *********** Create Contact "Contact Region 2" *********** Real Constant Set For Above Contact Is 8 & 7 *********** Create Contact "Contact Region 3" *********** Real Constant Set For Above Contact Is 10 & 9 *********** Send Named Selection as Node Component *********** *********** Send Named Selection as Node Component *********** *********** Send Named Selection as Node Component *********** *********** Send Named Selection as Element Component *********** *********** Fixed Supports *********** ********* Frictionless Supports X ********* *********** Node Rotations *********** *********** Create Remote Point "Remote Point" *********** *********** Construct Remote Force *********** *********** Define Body Force Temperature *********** ***** ROUTINE COMPLETED ***** CP = 0.525 --- Number of total nodes = 5853 --- Number of contact elements = 330 --- Number of spring elements = 0 --- Number of bearing elements = 0 --- Number of solid elements = 1120 --- Number of condensed parts = 0 --- Number of total elements = 1451 *GET _WALLBSOL FROM ACTI ITEM=TIME WALL VALUE= 14.8219444 **************************************************************************** ************************* SOLUTION ******************************** **************************************************************************** ***** MAPDL SOLUTION ROUTINE ***** PERFORM A STATIC ANALYSIS THIS WILL BE A NEW ANALYSIS PARAMETER _THICKRATIO = 1.000000000 USE PRECONDITIONED CONJUGATE GRADIENT SOLVER CONVERGENCE TOLERANCE = 1.00000E-08 MAXIMUM ITERATION = NumNode*DofPerNode* 1.0000 CONTACT INFORMATION PRINTOUT LEVEL 1 CHECK INITIAL OPEN/CLOSED STATUS OF SELECTED CONTACT ELEMENTS AND LIST DETAILED CONTACT PAIR INFORMATION SPLIT CONTACT SURFACES AT SOLVE PHASE NUMBER OF SPLITTING TBD BY PROGRAM DO NOT COMBINE ELEMENT MATRIX FILES (.emat) AFTER DISTRIBUTED PARALLEL SOLUTION DO NOT COMBINE ELEMENT SAVE DATA FILES (.esav) AFTER DISTRIBUTED PARALLEL SOLUTION NLDIAG: Nonlinear diagnostics CONT option is set to ON. Writing frequency : each ITERATION. DO NOT SAVE ANY RESTART FILES AT ALL **************************************************** ******************* SOLVE FOR LS 1 OF 1 **************** SELECT FOR ITEM=NODE COMPONENT= IN RANGE 5853 TO 5853 STEP 1 1 NODES (OF 5853 DEFINED) SELECTED BY NSEL COMMAND. SPECIFIED NODAL LOAD FX FOR SELECTED NODES 1 TO 5853 BY 1 REAL= 1.000000000E+10 IMAG= 0.00000000 SPECIFIED NODAL LOAD FY FOR SELECTED NODES 1 TO 5853 BY 1 REAL= 0.00000000 IMAG= 0.00000000 SPECIFIED NODAL LOAD FZ FOR SELECTED NODES 1 TO 5853 BY 1 REAL= 0.00000000 IMAG= 0.00000000 ALL SELECT FOR ITEM=NODE COMPONENT= IN RANGE 1 TO 5853 STEP 1 5853 NODES (OF 5853 DEFINED) SELECTED BY NSEL COMMAND. PRINTOUT RESUMED BY /GOP USE 1 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL DEGREES OF FREEDOM FOR AUTOMATIC TIME STEPPING: USE 1 SUBSTEPS AS A MAXIMUM USE 1 SUBSTEPS AS A MINIMUM TIME= 1.0000 ERASE THE CURRENT DATABASE OUTPUT CONTROL TABLE. WRITE ALL ITEMS TO THE DATABASE WITH A FREQUENCY OF NONE FOR ALL APPLICABLE ENTITIES WRITE NSOL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE RSOL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE EANG ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE ETMP ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE VENG ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE STRS ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE EPEL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE EPPL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE EPTH ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES WRITE CONT ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL FOR ALL APPLICABLE ENTITIES *GET ANSINTER_ FROM ACTI ITEM=INT VALUE= 0.00000000 *IF ANSINTER_ ( = 0.00000 ) NE 0 ( = 0.00000 ) THEN *ENDIF *** NOTE *** CP = 0.702 TIME= 14:49:19 The automatic domain decomposition logic has selected the MESH domain decomposition method with 4 processes per solution. ***** MAPDL SOLVE COMMAND ***** *** WARNING *** CP = 0.717 TIME= 14:49:19 Element shape checking is currently inactive. Issue SHPP,ON or SHPP,WARN to reactivate, if desired. *** NOTE *** CP = 0.739 TIME= 14:49:19 The model data was checked and warning messages were found. Please review output or errors file ( /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/fil le0.err ) for these warning messages. *** SELECTION OF ELEMENT TECHNOLOGIES FOR APPLICABLE ELEMENTS *** --- GIVE SUGGESTIONS AND RESET THE KEY OPTIONS --- ELEMENT TYPE 1 IS SOLID186. KEYOPT(2)=0 IS SUGGESTED AND HAS BEEN RESET. KEYOPT(1-12)= 0 0 0 0 0 0 0 0 0 0 0 0 ELEMENT TYPE 2 IS SOLID186. KEYOPT(2)=0 IS SUGGESTED AND HAS BEEN RESET. KEYOPT(1-12)= 0 0 0 0 0 0 0 0 0 0 0 0 ELEMENT TYPE 3 IS SOLID186. KEYOPT(2)=0 IS SUGGESTED AND HAS BEEN RESET. KEYOPT(1-12)= 0 0 0 0 0 0 0 0 0 0 0 0 ELEMENT TYPE 4 IS SOLID186. KEYOPT(2)=0 IS SUGGESTED AND HAS BEEN RESET. KEYOPT(1-12)= 0 0 0 0 0 0 0 0 0 0 0 0 *** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2024 R2 24.2 *** Ansys Mechanical Enterprise 00000000 VERSION=LINUX x64 14:49:19 NOV 04, 2024 CP= 0.741 --Static Structural S O L U T I O N O P T I O N S PROBLEM DIMENSIONALITY. . . . . . . . . . . . .3-D DEGREES OF FREEDOM. . . . . . UX UY UZ ROTX ROTY ROTZ ANALYSIS TYPE . . . . . . . . . . . . . . . . .STATIC (STEADY-STATE) OFFSET TEMPERATURE FROM ABSOLUTE ZERO . . . . . 273.15 EQUATION SOLVER OPTION. . . . . . . . . . . . .PCG TOLERANCE. . . . . . . . . . . . . . . . . . 1.00000E-08 GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC *** NOTE *** CP = 0.750 TIME= 14:49:19 The conditions for direct assembly have been met. No .emat or .erot files will be produced. TRIM CONTACT/TARGET SURFACE *** NOTE *** CP = 0.778 TIME= 14:49:19 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. *** NOTE *** CP = 0.801 TIME= 14:49:19 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. START TRIMMING SMALL/BONDED CONTACT PAIRS FOR DMP RUN. 76 CONTACT ELEMENTS & 76 TARGET ELEMENTS ARE DELETED DUE TO TRIMMING LOGIC. 3 CONTACT PAIRS ARE REMOVED. CHECK INITIAL OPEN/CLOSED STATUS OF SELECTED CONTACT ELEMENTS AND LIST DETAILED CONTACT PAIR INFORMATION *** NOTE *** CP = 1.115 TIME= 14:49:19 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. *** NOTE *** CP = 1.124 TIME= 14:49:19 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. *** NOTE *** CP = 1.147 TIME= 14:49:20 The maximum number of contact elements in any single contact pair is 26, which is smaller than the optimal domain size of 120 elements for the given number of CPU domains (4). Therefore, no contact pairs are being split by the CNCH,DMP logic. *** NOTE *** CP = 1.151 TIME= 14:49:20 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. *** NOTE *** CP = 1.159 TIME= 14:49:20 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. *** NOTE *** CP = 1.232 TIME= 14:49:20 Deformable-deformable contact pair identified by real constant set 5 and contact element type 5 has been set up. Linear contact is defined Contact algorithm: Augmented Lagrange method Contact detection at: Gauss integration point Contact stiffness factor FKN 10.000 The resulting initial contact stiffness 0.10000E+15 Default penetration tolerance factor FTOLN 0.10000 The resulting penetration tolerance 0.40000E-01 Default opening contact stiffness OPSF will be used. Default tangent stiffness factor FKT 1.0000 Use constant contact stiffness Default Max. friction stress TAUMAX 0.10000E+21 Average contact surface length 0.35821 Average contact pair depth 0.40000 Average target surface length 0.34527 Default pinball region factor PINB 0.25000 The resulting pinball region 0.10000 Initial penetration/gap is excluded. Bonded contact (always) is defined. *** NOTE *** CP = 1.232 TIME= 14:49:20 Max. Initial penetration 4.440892099E-16 was detected between contact element 1965 and target element 2013. **************************************** *** NOTE *** CP = 1.233 TIME= 14:49:20 Deformable-deformable contact pair identified by real constant set 7 and contact element type 7 has been set up. Linear contact is defined Contact algorithm: Augmented Lagrange method Contact detection at: Gauss integration point Contact stiffness factor FKN 10.000 The resulting initial contact stiffness 0.88000E+14 Default penetration tolerance factor FTOLN 0.10000 The resulting penetration tolerance 0.45455E-01 Default opening contact stiffness OPSF will be used. Default tangent stiffness factor FKT 1.0000 Use constant contact stiffness Default Max. friction stress TAUMAX 0.10000E+21 Average contact surface length 0.35806 Average contact pair depth 0.45455 Average target surface length 0.34573 Default pinball region factor PINB 0.25000 The resulting pinball region 0.11364 Initial penetration/gap is excluded. Bonded contact (always) is defined. *** NOTE *** CP = 1.233 TIME= 14:49:20 Max. Initial penetration 1.776356839E-15 was detected between contact element 2072 and target element 2126. **************************************** *** NOTE *** CP = 1.233 TIME= 14:49:20 Deformable-deformable contact pair identified by real constant set 9 and contact element type 9 has been set up. Linear contact is defined Contact algorithm: Augmented Lagrange method Contact detection at: Gauss integration point Contact stiffness factor FKN 10.000 The resulting initial contact stiffness 0.84000E+14 Default penetration tolerance factor FTOLN 0.10000 The resulting penetration tolerance 0.47619E-01 Default opening contact stiffness OPSF will be used. Default tangent stiffness factor FKT 1.0000 Use constant contact stiffness Default Max. friction stress TAUMAX 0.10000E+21 Average contact surface length 0.33559 Average contact pair depth 0.47619 Average target surface length 0.36304 Default pinball region factor PINB 0.25000 The resulting pinball region 0.11905 Initial penetration/gap is excluded. Bonded contact (always) is defined. *** NOTE *** CP = 1.234 TIME= 14:49:20 Max. Initial penetration 3.552713679E-15 was detected between contact element 2171 and target element 2222. **************************************** *** NOTE *** CP = 1.234 TIME= 14:49:20 Force-distributed-surface identified by real constant set 11 and contact element type 11 has been set up. The pilot node 5853 is used to apply the force. Internal MPC will be built. The used degrees of freedom set is UX UY UZ ROTX ROTY ROTZ Please verify constraints (including rotational degrees of freedom) on the pilot node by yourself. **************************************** *** NOTE *** CP = 1.240 TIME= 14:49:20 Internal nodes from 5854 to 5854 are created. 1 internal nodes are used for handling degrees of freedom on pilot nodes of rigid target surfaces. D I S T R I B U T E D D O M A I N D E C O M P O S E R ...Number of elements: 1299 ...Number of nodes: 5854 ...Decompose to 4 CPU domains ...Element load balance ratio = 1.029 L O A D S T E P O P T I O N S LOAD STEP NUMBER. . . . . . . . . . . . . . . . 1 TIME AT END OF THE LOAD STEP. . . . . . . . . . 1.0000 NUMBER OF SUBSTEPS. . . . . . . . . . . . . . . 1 STEP CHANGE BOUNDARY CONDITIONS . . . . . . . . NO PRINT OUTPUT CONTROLS . . . . . . . . . . . . .NO PRINTOUT DATABASE OUTPUT CONTROLS ITEM FREQUENCY COMPONENT ALL NONE NSOL ALL RSOL ALL EANG ALL ETMP ALL VENG ALL STRS ALL EPEL ALL EPPL ALL EPTH ALL CONT ALL SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr *** NOTE *** CP = 1.653 TIME= 14:49:20 The PCG solver has automatically set the level of difficulty for this model to 2. *********** PRECISE MASS SUMMARY *********** TOTAL RIGID BODY MASS MATRIX ABOUT ORIGIN Translational mass | Coupled translational/rotational mass 0.49319E+06 0.0000 0.0000 | 0.0000 0.71581E-03 -0.99840E-03 0.0000 0.49319E+06 0.0000 | -0.71581E-03 0.0000 0.49319E+07 0.0000 0.0000 0.49319E+06 | 0.99840E-03 -0.49319E+07 0.0000 ------------------------------------------ | ------------------------------------------ | Rotational mass (inertia) | 0.24657E+06 -0.10441E-01 -0.84927E-02 | -0.10441E-01 0.65882E+08 0.38797E-02 | -0.84927E-02 0.38797E-02 0.65882E+08 TOTAL MASS = 0.49319E+06 The mass principal axes coincide with the global Cartesian axes CENTER OF MASS (X,Y,Z)= 10.000 0.20244E-08 0.14514E-08 TOTAL INERTIA ABOUT CENTER OF MASS 0.24657E+06 -0.45689E-03 -0.13346E-02 -0.45689E-03 0.16563E+08 0.38797E-02 -0.13346E-02 0.38797E-02 0.16563E+08 The inertia principal axes coincide with the global Cartesian axes *** MASS SUMMARY BY ELEMENT TYPE *** TYPE MASS 1 49318.9 2 123297. 3 246594. 4 73978.3 Range of element maximum matrix coefficients in global coordinates Maximum = 4.56569776E+12 at element 2188. Minimum = 7.008802843E+10 at element 81. *** ELEMENT MATRIX FORMULATION TIMES TYPE NUMBER ENAME TOTAL CP AVE CP 1 120 SOLID186 0.035 0.000288 2 286 SOLID186 0.078 0.000274 3 546 SOLID186 0.275 0.000503 4 168 SOLID186 0.051 0.000304 5 24 CONTA174 0.013 0.000525 6 26 TARGE170 0.000 0.000002 7 26 CONTA174 0.014 0.000527 8 26 TARGE170 0.000 0.000003 9 26 CONTA174 0.010 0.000377 10 24 TARGE170 0.000 0.000002 11 26 CONTA174 0.000 0.000007 12 1 TARGE170 0.000 0.000008 Time at end of element matrix formulation CP = 2.07581782. Iteration= 5 Ratio= 0.261817 Limit= 1.000000E-08 Wall= 0.0 Iteration= 50 Ratio= 7.069725E-04 Limit= 1.000000E-08 Wall= 0.0 Iteration= 140 Ratio= 2.040034E-06 Limit= 1.000000E-08 Wall= 0.1 DISTRIBUTED PCG SOLVER SOLUTION CONVERGED DISTRIBUTED PCG SOLVER SOLUTION STATISTICS NUMBER OF ITERATIONS= 221 NUMBER OF EQUATIONS = 17568 LEVEL OF CONVERGENCE= 1 CALCULATED NORM = 0.96418E-08 SPECIFIED TOLERANCE = 0.10000E-07 TOTAL CPU TIME (sec)= 0.17 TOTAL WALL TIME(sec)= 0.17 TOTAL MEMORY (GB) = 0.02 *** ELEMENT RESULT CALCULATION TIMES TYPE NUMBER ENAME TOTAL CP AVE CP 1 120 SOLID186 0.013 0.000107 2 286 SOLID186 0.029 0.000101 3 546 SOLID186 0.055 0.000100 4 168 SOLID186 0.017 0.000102 5 24 CONTA174 0.002 0.000081 7 26 CONTA174 0.002 0.000083 9 26 CONTA174 0.002 0.000076 11 26 CONTA174 0.000 0.000002 *** NODAL LOAD CALCULATION TIMES TYPE NUMBER ENAME TOTAL CP AVE CP 1 120 SOLID186 0.002 0.000018 2 286 SOLID186 0.005 0.000017 3 546 SOLID186 0.009 0.000017 4 168 SOLID186 0.003 0.000017 5 24 CONTA174 0.000 0.000017 7 26 CONTA174 0.001 0.000024 9 26 CONTA174 0.000 0.000016 11 26 CONTA174 0.000 0.000000 *** LOAD STEP 1 SUBSTEP 1 COMPLETED. CUM ITER = 1 *** TIME = 1.00000 TIME INC = 1.00000 NEW TRIANG MATRIX *** MAPDL BINARY FILE STATISTICS BUFFER SIZE USED= 16384 0.562 MB WRITTEN ON ELEMENT SAVED DATA FILE: file0.esav 0.750 MB WRITTEN ON RESULTS FILE: file0.rst *************** Write FE CONNECTORS ********* WRITE OUT CONSTRAINT EQUATIONS TO FILE= file.ce **************************************************** *************** FINISHED SOLVE FOR LS 1 ************* *GET _WALLASOL FROM ACTI ITEM=TIME WALL VALUE= 14.8222222 PRINTOUT RESUMED BY /GOP *GET _PCGITER FROM ACTI ITEM=SOLU CGIT VALUE= 221.000000 FINISH SOLUTION PROCESSING ***** ROUTINE COMPLETED ***** CP = 2.335 *** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2024 R2 24.2 *** Ansys Mechanical Enterprise 00000000 VERSION=LINUX x64 14:49:20 NOV 04, 2024 CP= 2.337 --Static Structural ***** MAPDL RESULTS INTERPRETATION (POST1) ***** *** NOTE *** CP = 2.337 TIME= 14:49:20 Reading results into the database (SET command) will update the current displacement and force boundary conditions in the database with the values from the results file for that load set. Note that any subsequent solutions will use these values unless action is taken to either SAVE the current values or not overwrite them (/EXIT,NOSAVE). Set Encoding of XML File to:ISO-8859-1 Set Output of XML File to: PARM, , , , , , , , , , , , , , , , , , , DATABASE WRITTEN ON FILE parm.xml EXIT THE MAPDL POST1 DATABASE PROCESSOR ***** ROUTINE COMPLETED ***** CP = 2.340 PRINTOUT RESUMED BY /GOP *GET _WALLDONE FROM ACTI ITEM=TIME WALL VALUE= 14.8222222 PARAMETER _PREPTIME = 0.000000000 PARAMETER _SOLVTIME = 1.000000000 PARAMETER _POSTTIME = 0.000000000 PARAMETER _TOTALTIM = 1.000000000 *GET _DLBRATIO FROM ACTI ITEM=SOLU DLBR VALUE= 1.02931596 *GET _COMBTIME FROM ACTI ITEM=SOLU COMB VALUE= 0.718758517E-02 *GET _SSMODE FROM ACTI ITEM=SOLU SSMM VALUE= 0.00000000 *GET _NDOFS FROM ACTI ITEM=SOLU NDOF VALUE= 15136.0000 *GET _SOL_END_TIME FROM ACTI ITEM=SET TIME VALUE= 1.00000000 *IF _sol_end_time ( = 1.00000 ) EQ 1.000000 ( = 1.00000 ) THEN /FCLEAN COMMAND REMOVING ALL LOCAL FILES *ENDIF --- Total number of nodes = 5853 --- Total number of elements = 1299 --- Element load balance ratio = 1.02931596 --- Time to combine distributed files = 7.187585167E-03 --- Sparse memory mode = 0 --- Number of DOF = 15136 EXIT MAPDL WITHOUT SAVING DATABASE NUMBER OF WARNING MESSAGES ENCOUNTERED= 2 NUMBER OF ERROR MESSAGES ENCOUNTERED= 0 +--------------------- M A P D L S T A T I S T I C S ------------------------+ Release: 2024 R2 Build: 24.2 Update: UP20240603 Platform: LINUX x64 Date Run: 11/04/2024 Time: 14:49 Process ID: 1499 Operating System: Ubuntu 20.04.6 LTS Processor Model: AMD EPYC 7763 64-Core Processor Compiler: Intel(R) Fortran Compiler Classic Version 2021.9 (Build: 20230302) Intel(R) C/C++ Compiler Classic Version 2021.9 (Build: 20230302) AOCL-BLAS 4.2.1 Build 20240303 Number of machines requested : 1 Total number of cores available : 8 Number of physical cores available : 4 Number of processes requested : 4 Number of threads per process requested : 1 Total number of cores requested : 4 (Distributed Memory Parallel) MPI Type: INTELMPI MPI Version: Intel(R) MPI Library 2021.11 for Linux* OS GPU Acceleration: Not Requested Job Name: file0 Input File: dummy.dat Core Machine Name Working Directory ----------------------------------------------------- 0 938793e4e167 /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural 1 938793e4e167 /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural 2 938793e4e167 /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural 3 938793e4e167 /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural Latency time from master to core 1 = 2.253 microseconds Latency time from master to core 2 = 2.754 microseconds Latency time from master to core 3 = 2.142 microseconds Communication speed from master to core 1 = 9835.90 MB/sec Communication speed from master to core 2 = 14498.48 MB/sec Communication speed from master to core 3 = 14864.79 MB/sec Total CPU time for main thread : 1.2 seconds Total CPU time summed for all threads : 3.0 seconds Elapsed time spent obtaining a license : 0.4 seconds Elapsed time spent pre-processing model (/PREP7) : 0.0 seconds Elapsed time spent solution - preprocessing : 0.2 seconds Elapsed time spent computing solution : 0.4 seconds Elapsed time spent solution - postprocessing : 0.0 seconds Elapsed time spent post-processing model (/POST1) : 0.0 seconds Equation solver used : PCG (symmetric) Equation solver computational rate : 26.1 Gflops Sum of disk space used on all processes : 17.6 MB Sum of memory used on all processes : 223.0 MB Sum of memory allocated on all processes : 2880.0 MB Physical memory available : 31 GB Total amount of I/O written to disk : 0.0 GB Total amount of I/O read from disk : 0.0 GB +------------------ E N D M A P D L S T A T I S T I C S -------------------+ *-----------------------------------------------------------------------------* | | | RUN COMPLETED | | | |-----------------------------------------------------------------------------| | | | Ansys MAPDL 2024 R2 Build 24.2 UP20240603 LINUX x64 | | | |-----------------------------------------------------------------------------| | | | Database Requested(-db) 1024 MB Scratch Memory Requested 1024 MB | | Max Database Used(Master) 6 MB Max Scratch Used(Master) 61 MB | | Max Database Used(Workers) 1 MB Max Scratch Used(Workers) 51 MB | | Sum Database Used(All) 9 MB Sum Scratch Used(All) 214 MB | | | |-----------------------------------------------------------------------------| | | | CP Time (sec) = 2.964 Time = 14:49:21 | | Elapsed Time (sec) = 4.000 Date = 11/04/2024 | | | *-----------------------------------------------------------------------------* .. GENERATED FROM PYTHON SOURCE LINES 213-216 Close Mechanical ~~~~~~~~~~~~~~~~ Close the Mechanical session. .. GENERATED FROM PYTHON SOURCE LINES 216-218 .. code-block:: Python mechanical.exit() .. rst-class:: sphx-glr-timing **Total running time of the script:** (0 minutes 19.183 seconds) .. _sphx_glr_download_examples_00_basic_example_01_simple_structural_solve.py: .. only:: html .. container:: sphx-glr-footer sphx-glr-footer-example .. container:: sphx-glr-download sphx-glr-download-jupyter :download:`Download Jupyter notebook: example_01_simple_structural_solve.ipynb ` .. container:: sphx-glr-download sphx-glr-download-python :download:`Download Python source code: example_01_simple_structural_solve.py ` .. container:: sphx-glr-download sphx-glr-download-zip :download:`Download zipped: example_01_simple_structural_solve.zip ` .. only:: html .. rst-class:: sphx-glr-signature `Gallery generated by Sphinx-Gallery `_