Note
Go to the end to download the full example code.
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.
Download required files#
Download the required files. Print the file path for the geometry file.
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}")
Downloaded the geometry file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_01_geometry.agdb
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.
mechanical = launch_mechanical(batch=True, cleanup_on_exit=False)
print(mechanical)
Ansys Mechanical [Ansys Mechanical Enterprise]
Product Version:242
Software build date: 06/03/2024 09:35:09
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.
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}")
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<?, ?B/s]
Uploading example_01_geometry.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/.: 100%|██████████| 17.0k/17.0k [00:00<00:00, 63.6MB/s]
part_file_path on server: /tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/example_01_geometry.agdb
Run the script#
Run the Mechanical script to attach the geometry and set up and solve the analysis.
output = mechanical.run_python_script(
"""
import json
# Section 1: Read geometry information
geometry_import_group_11 = Model.GeometryImportGroup
geometry_import_19 = geometry_import_group_11.AddGeometryImport()
geometry_import_19_format = Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.\
Format.Automatic
geometry_import_19_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
geometry_import_19_preferences.ProcessNamedSelections = True
geometry_import_19_preferences.ProcessCoordinateSystems = True
geometry_import_19.Import(part_file_path, geometry_import_19_format, geometry_import_19_preferences)
Model.AddStaticStructuralAnalysis()
STAT_STRUC = Model.Analyses[0]
CS_GRP = Model.CoordinateSystems
ANALYSIS_SETTINGS = STAT_STRUC.Children[0]
SOLN= STAT_STRUC.Solution
# Section 2: Set up the unit system.
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS
ExtAPI.Application.ActiveAngleUnit = AngleUnitType.Radian
# Section 3: Define named selection and coordinate system.
NS1 = Model.NamedSelections.Children[0]
NS2 = Model.NamedSelections.Children[1]
NS3 = Model.NamedSelections.Children[2]
NS4 = Model.NamedSelections.Children[3]
GCS = CS_GRP.Children[0]
LCS1 = CS_GRP.Children[1]
# Section 4: Define remote point.
RMPT_GRP = Model.RemotePoints
RMPT_1 = RMPT_GRP.AddRemotePoint()
RMPT_1.Location = NS1
RMPT_1.XCoordinate=Quantity("7 [m]")
RMPT_1.YCoordinate=Quantity("0 [m]")
RMPT_1.ZCoordinate=Quantity("0 [m]")
# Section 5: Define mesh settings.
MSH = Model.Mesh
MSH.ElementSize =Quantity("0.5 [m]")
MSH.GenerateMesh()
# Section 6: Define boundary conditions.
# Insert fixed support.
FIX_SUP = STAT_STRUC.AddFixedSupport()
FIX_SUP.Location = NS2
# Insert frictionless support.
FRIC_SUP = STAT_STRUC.AddFrictionlessSupport()
FRIC_SUP.Location = NS3
# Section 7: Define remote force.
REM_FRC1 = STAT_STRUC.AddRemoteForce()
REM_FRC1.Location = RMPT_1
REM_FRC1.DefineBy =LoadDefineBy.Components
REM_FRC1.XComponent.Output.DiscreteValues = [Quantity("1e10 [N]")]
# Section 8: Define thermal condition.
THERM_COND = STAT_STRUC.AddThermalCondition()
THERM_COND.Location = NS4
THERM_COND.Magnitude.Output.DefinitionType=VariableDefinitionType.Formula
THERM_COND.Magnitude.Output.Formula="50*(20+z)"
THERM_COND.XYZFunctionCoordinateSystem=LCS1
THERM_COND.RangeMinimum=Quantity("-20 [m]")
THERM_COND.RangeMaximum=Quantity("1 [m]")
# Section 9: Insert directional deformation.
DIR_DEF = STAT_STRUC.Solution.AddDirectionalDeformation()
DIR_DEF.Location = NS1
DIR_DEF.NormalOrientation =NormalOrientationType.XAxis
# Section 10: Add total deformation and force reaction probe.
TOT_DEF = STAT_STRUC.Solution.AddTotalDeformation()
# Add force reaction.
FRC_REAC_PROBE = STAT_STRUC.Solution.AddForceReaction()
FRC_REAC_PROBE.BoundaryConditionSelection = FIX_SUP
FRC_REAC_PROBE.ResultSelection =ProbeDisplayFilter.XAxis
# Section 11: Solve and get the results.
# Solve static analysis.
STAT_STRUC.Solution.Solve(True)
dir_deformation_details = {
"Minimum": str(DIR_DEF.Minimum),
"Maximum": str(DIR_DEF.Maximum),
"Average": str(DIR_DEF.Average),
}
json.dumps(dir_deformation_details)
"""
)
print(output)
{"Maximum": "0.10480765998363495 [m]", "Minimum": "0.10404198616743088 [m]", "Average": "0.10450294822133997 [m]"}
Download output file from solve and print contents#
Download the solve.out file from the server to the current working
directory and print the contents. Remove the solve.out file.
def get_solve_out_path(mechanical):
solve_out_path = ""
for file_path in mechanical.list_files():
if file_path.find("solve.out") != -1:
solve_out_path = file_path
break
return solve_out_path
def write_file_contents_to_console(path):
with open(path, "rt") as file:
for line in file:
print(line, end="")
solve_out_path = get_solve_out_path(mechanical)
if solve_out_path != "":
current_working_directory = os.getcwd()
local_file_path_list = mechanical.download(
solve_out_path, target_dir=current_working_directory
)
solve_out_local_path = local_file_path_list[0]
print(f"Local solve.out path : {solve_out_local_path}")
write_file_contents_to_console(solve_out_local_path)
os.remove(solve_out_local_path)
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/solve.out to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/00_basic/solve.out: 0%| | 0.00/36.8k [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech6190/Project_Mech_Files/StaticStructural/solve.out to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/00_basic/solve.out: 100%|██████████| 36.8k/36.8k [00:00<00:00, 198MB/s]
Local solve.out path : /home/runner/work/pymechanical-examples/pymechanical-examples/examples/00_basic/solve.out
Ansys Mechanical Enterprise
*------------------------------------------------------------------*
| |
| W E L C O M E T O T H E A N S Y S (R) P R O G R A M |
| |
*------------------------------------------------------------------*
***************************************************************
* ANSYS MAPDL 2024 R2 LEGAL NOTICES *
***************************************************************
* *
* Copyright 1971-2024 Ansys, Inc. All rights reserved. *
* Unauthorized use, distribution or duplication is *
* prohibited. *
* *
* Ansys is a registered trademark of Ansys, Inc. or its *
* subsidiaries in the United States or other countries. *
* See the Ansys, Inc. online documentation or the Ansys, Inc. *
* documentation CD or online help for the complete Legal *
* Notice. *
* *
***************************************************************
* *
* THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION *
* INCLUDE TRADE SECRETS AND CONFIDENTIAL AND PROPRIETARY *
* PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. *
* The software products and documentation are furnished by *
* Ansys, Inc. or its subsidiaries under a software license *
* agreement that contains provisions concerning *
* non-disclosure, copying, length and nature of use, *
* compliance with exporting laws, warranties, disclaimers, *
* limitations of liability, and remedies, and other *
* provisions. The software products and documentation may be *
* used, disclosed, transferred, or copied only in accordance *
* with the terms and conditions of that software license *
* agreement. *
* *
* Ansys, Inc. is a UL registered *
* ISO 9001:2015 company. *
* *
***************************************************************
* *
* This product is subject to U.S. laws governing export and *
* re-export. *
* *
* For U.S. Government users, except as specifically granted *
* by the Ansys, Inc. software license agreement, the use, *
* duplication, or disclosure by the United States Government *
* is subject to restrictions stated in the Ansys, Inc. *
* software license agreement and FAR 12.212 (for non-DOD *
* licenses). *
* *
***************************************************************
*------------------------------------------------------------------*
| Ansys Product Improvement |
| |
| Ansys Product Improvement Program helps improve Ansys |
| products. Participating in this program is like filling out a |
| survey. Without interrupting your work, the software reports |
| anonymous usage information such as errors, machine and |
| solver statistics, features used, etc. to Ansys. We never |
| use the data to identify or contact you. |
| The data does NOT contain: |
| - Any personally identifiable information including names, |
| IP addresses, file names, part names, etc. |
| - Any information about your geometry or design specific |
| inputs. |
| You can stop participation at any time. To change your |
| selection go to Help >> 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 |
| |
*-----------------------------------------------------------------------------*
Close Mechanical#
Close the Mechanical session.
mechanical.exit()
Total running time of the script: (0 minutes 19.183 seconds)