Bolt Pretension#

This example demonstrates how to insert a Static Structural analysis into a new Mechanical session and execute a sequence of Python scripting commands that define and solve a bolt-pretension analysis. Scripts then evaluate the following results: deformation, equivalent stresses, contact, and bolt

Import necessary libraries#

import os

from ansys.mechanical.core import launch_mechanical
from ansys.mechanical.core.examples import download_file
from matplotlib import image as mpimg
from matplotlib import pyplot as plt

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:251
Software build date: 11/27/2024 09:34:44

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}")
project directory = /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/

Download required geometry file#

Download the required file. Print the file path for the geometry file.

geometry_path = download_file(
    "example_06_bolt_pret_geom.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_06_bolt_pret_geom.agdb

Upload the file to the project directory

mechanical.upload(file_name=geometry_path, file_location_destination=project_directory)
Uploading example_06_bolt_pret_geom.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.:   0%|          | 0.00/2.52M [00:00<?, ?B/s]
Uploading example_06_bolt_pret_geom.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.: 100%|██████████| 2.52M/2.52M [00:00<00:00, 414MB/s]

'example_06_bolt_pret_geom.agdb'

Build the path relative to project directory and verify

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}'")
result = mechanical.run_python_script("part_file_path")
print(f"Geometry file on server: {result}")
Geometry file on server: /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/example_06_bolt_pret_geom.agdb

Download required material file#

Download the required file. Print the file path for the material file

mat_cop_path = download_file("example_06_Mat_Copper.xml", "pymechanical", "00_basic")
print(f"Downloaded the material file to: {mat_cop_path}")
mat_st_path = download_file("example_06_Mat_Steel.xml", "pymechanical", "00_basic")
print(f"Downloaded the material file to: {mat_st_path}")
Downloaded the material file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_06_Mat_Copper.xml
Downloaded the material file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_06_Mat_Steel.xml

Upload the file to the project directory

mechanical.upload(file_name=mat_cop_path, file_location_destination=project_directory)
mechanical.upload(file_name=mat_st_path, file_location_destination=project_directory)
Uploading example_06_Mat_Copper.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.:   0%|          | 0.00/5.00k [00:00<?, ?B/s]
Uploading example_06_Mat_Copper.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.: 100%|██████████| 5.00k/5.00k [00:00<00:00, 16.9MB/s]

Uploading example_06_Mat_Steel.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.:   0%|          | 0.00/5.00k [00:00<?, ?B/s]
Uploading example_06_Mat_Steel.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/.: 100%|██████████| 5.00k/5.00k [00:00<00:00, 24.7MB/s]

'example_06_Mat_Steel.xml'

Build the path relative to project directory and verify

base_name = os.path.basename(mat_cop_path)
combined_path = os.path.join(project_directory, base_name)
mat_Copper_file_path = combined_path.replace("\\", "\\\\")
mechanical.run_python_script(f"mat_Copper_file_path='{mat_Copper_file_path}'")

base_name = os.path.basename(mat_st_path)
combined_path = os.path.join(project_directory, base_name)
mat_Steel_file_path = combined_path.replace("\\", "\\\\")
mechanical.run_python_script(f"mat_Steel_file_path='{mat_Steel_file_path}'")

result = mechanical.run_python_script("mat_Copper_file_path")
print(f"mat_Copper_file_path on server: {result}")
result = mechanical.run_python_script("mat_Steel_file_path")
print(f"mat_Steel_file_path on server: {result}")
mat_Copper_file_path on server: /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/example_06_Mat_Copper.xml
mat_Steel_file_path on server: /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/example_06_Mat_Steel.xml

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
import os

# Read geometry and material information.
geometry_import_group = Model.GeometryImportGroup
geometry_import = geometry_import_group.AddGeometryImport()
geometry_import_format = Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.\
    Format.Automatic
geometry_import_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
geometry_import_preferences.ProcessNamedSelections = True
geometry_import_preferences.ProcessCoordinateSystems = True
geometry_import.Import(part_file_path,geometry_import_format,geometry_import_preferences)

# Import materials.
MAT = ExtAPI.DataModel.Project.Model.Materials
MAT.Import(mat_Copper_file_path)
MAT.Import(mat_Steel_file_path)

Model.AddStaticStructuralAnalysis()
STAT_STRUC = Model.Analyses[0]
STAT_STRUC_SOLN = STAT_STRUC.Solution
STAT_STRUC_ANA_SETTING = STAT_STRUC.Children[0]

# Set up the unit system.
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMM

# Store all main tree nodes as variables.
MODEL = ExtAPI.DataModel.Project.Model
GEOM = ExtAPI.DataModel.Project.Model.Geometry
CONN_GRP = ExtAPI.DataModel.Project.Model.Connections
CS_GRP = ExtAPI.DataModel.Project.Model.CoordinateSystems
MSH = ExtAPI.DataModel.Project.Model.Mesh
NS_GRP = ExtAPI.DataModel.Project.Model.NamedSelections

# Store name selection.
block3_block2_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block3_block2_cont'][0]
block3_block2_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block3_block2_targ'][0]
shank_block3_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_block3_targ'][0]
shank_block3_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_block3_cont'][0]
block1_washer_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block1_washer_cont'][0]
block1_washer_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block1_washer_targ'][0]
washer_bolt_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'washer_bolt_cont'][0]
washer_bolt_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'washer_bolt_targ'][0]
shank_bolt_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_bolt_targ'][0]
shank_bolt_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_bolt_cont'][0]
block2_block1_cont_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block2_block1_cont'][0]
block2_block1_targ_NS = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block2_block1_targ'][0]
all_bodies = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'all_bodies'][0]
bodies_5 = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'bodies_5'][0]
shank = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank'][0]
shank_face = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_face'][0]
shank_face2 = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_face2'][0]
bottom_surface = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'bottom_surface'][0]
block2_surface = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'block2_surface'][0]
shank_surface = [x for x in ExtAPI.DataModel.Tree.AllObjects
if x.Name == 'shank_surface'][0]

# Assign material to bodies.
SURFACE1=GEOM.Children[0].Children[0]
SURFACE1.Material="Steel"

SURFACE2=GEOM.Children[1].Children[0]
SURFACE2.Material="Copper"

SURFACE3=GEOM.Children[2].Children[0]
SURFACE3.Material="Copper"

SURFACE4=GEOM.Children[3].Children[0]
SURFACE4.Material="Steel"

SURFACE5=GEOM.Children[4].Children[0]
SURFACE5.Material="Steel"

SURFACE6=GEOM.Children[5].Children[0]
SURFACE6.Material="Steel"

# Define coordinate system.
coordinate_systems_17 = Model.CoordinateSystems
coordinate_system_93 = coordinate_systems_17.AddCoordinateSystem()
coordinate_system_93.OriginDefineBy = CoordinateSystemAlignmentType.Fixed
coordinate_system_93.OriginX = Quantity(-195, "mm")
coordinate_system_93.OriginY = Quantity(100, "mm")
coordinate_system_93.OriginZ = Quantity(50, "mm")
coordinate_system_93.PrimaryAxis = CoordinateSystemAxisType.PositiveZAxis

# Change contact settings and add a command snippet to use the Archard Wear Model.
connections =  ExtAPI.DataModel.Project.Model.Connections

# Delete existing contacts.
for connection in connections.Children:
    if connection.DataModelObjectCategory==DataModelObjectCategory.ConnectionGroup:
        connection.Delete()

CONT_REG1 = CONN_GRP.AddContactRegion()
CONT_REG1.SourceLocation = NS_GRP.Children[0]
CONT_REG1.TargetLocation = NS_GRP.Children[1]
CONT_REG1.ContactType=ContactType.Frictional
CONT_REG1.FrictionCoefficient = 0.2
CONT_REG1.SmallSliding = ContactSmallSlidingType.Off
CONT_REG1.UpdateStiffness = UpdateContactStiffness.Never
CMD1=CONT_REG1.AddCommandSnippet()

# Add missing contact keyopt and Archard Wear Model in workbench using a command snippet.
AWM = '''keyopt,cid,9,5
rmodif,cid,10,0.00
rmodif,cid,23,0.001'''
CMD1.AppendText(AWM)

CONTS = CONN_GRP.Children[0]
CONT_REG2 = CONTS.AddContactRegion()
CONT_REG2.SourceLocation = NS_GRP.Children[3]
CONT_REG2.TargetLocation = NS_GRP.Children[2]
CONT_REG2.ContactType=ContactType.Bonded
CONT_REG2.ContactFormulation = ContactFormulation.MPC

CONT_REG3 = CONTS.AddContactRegion()
CONT_REG3.SourceLocation = NS_GRP.Children[4]
CONT_REG3.TargetLocation = NS_GRP.Children[5]
CONT_REG3.ContactType=ContactType.Frictional
CONT_REG3.FrictionCoefficient = 0.2
CONT_REG3.SmallSliding = ContactSmallSlidingType.Off
CONT_REG3.UpdateStiffness = UpdateContactStiffness.Never
CMD3=CONT_REG3.AddCommandSnippet()

# Add missing contact keyopt and Archard Wear Model in workbench using a command snippet.
AWM3 = '''keyopt,cid,9,5
rmodif,cid,10,0.00
rmodif,cid,23,0.001'''
CMD3.AppendText(AWM3)

CONT_REG4 = CONTS.AddContactRegion()
CONT_REG4.SourceLocation = NS_GRP.Children[6]
CONT_REG4.TargetLocation = NS_GRP.Children[7]
CONT_REG4.ContactType=ContactType.Bonded
CONT_REG4.ContactFormulation = ContactFormulation.MPC

CONT_REG5 = CONTS.AddContactRegion()
CONT_REG5.SourceLocation = NS_GRP.Children[9]
CONT_REG5.TargetLocation = NS_GRP.Children[8]
CONT_REG5.ContactType=ContactType.Bonded
CONT_REG5.ContactFormulation = ContactFormulation.MPC

CONT_REG6 = CONTS.AddContactRegion()
CONT_REG6.SourceLocation = NS_GRP.Children[10]
CONT_REG6.TargetLocation = NS_GRP.Children[11]
CONT_REG6.ContactType=ContactType.Frictional
CONT_REG6.FrictionCoefficient = 0.2
CONT_REG6.SmallSliding = ContactSmallSlidingType.Off
CONT_REG6.UpdateStiffness = UpdateContactStiffness.Never
CMD6=CONT_REG6.AddCommandSnippet()
# Add missing contact keyopt and Archard Wear Model in workbench using a command snippet.
AWM6 = '''keyopt,cid,9,5
rmodif,cid,10,0.00
rmodif,cid,23,0.001'''
CMD6.AppendText(AWM6)

# Add contact tool.
#CONT_TOOL = CONN_GRP.AddContactTool()
#CONT_TOOL.AddPenetration()
#CONT_TOOL.AddStatus()
#CONT_TOOL.GenerateInitialContactResults()

# Generate mesh.

Hex_Method = MSH.AddAutomaticMethod()
Hex_Method.Location = all_bodies
Hex_Method.Method = MethodType.HexDominant

BODY_SIZING1=MSH.AddSizing()
BODY_SIZING1.Location=bodies_5
BODY_SIZING1.ElementSize = Quantity(15, "mm")

BODY_SIZING2=MSH.AddSizing()
BODY_SIZING2.Location=shank
BODY_SIZING2.ElementSize = Quantity(7, "mm")

Face_Meshing = MSH.AddFaceMeshing()
Face_Meshing.Location = shank_face
Face_Meshing.MappedMesh = False

Sweep_Method = MSH.AddAutomaticMethod()
Sweep_Method.Location = shank
Sweep_Method.Method = MethodType.Sweep
Sweep_Method.SourceTargetSelection = 2
Sweep_Method.SourceLocation = shank_face
Sweep_Method.TargetLocation = shank_face2

MSH.GenerateMesh()

# Set up analysis settings.
STAT_STRUC_ANA_SETTING.NumberOfSteps = 4
step_index_list = [1]
with Transaction():
    for step_index in step_index_list:
        STAT_STRUC_ANA_SETTING.SetAutomaticTimeStepping(step_index, AutomaticTimeStepping.Off)
STAT_STRUC_ANA_SETTING.Activate()
step_index_list = [1]
with Transaction():
    for step_index in step_index_list:
        STAT_STRUC_ANA_SETTING.SetNumberOfSubSteps(step_index, 2)
STAT_STRUC_ANA_SETTING.Activate()
STAT_STRUC_ANA_SETTING.SolverType = SolverType.Direct
STAT_STRUC_ANA_SETTING.SolverPivotChecking = SolverPivotChecking.Off


# Insert loading and BC.
FIX_SUP=STAT_STRUC.AddFixedSupport()
FIX_SUP.Location=block2_surface

Tabular_Force = STAT_STRUC.AddForce()
Tabular_Force.Location = bottom_surface
Tabular_Force.DefineBy = LoadDefineBy.Components
Tabular_Force.XComponent.Inputs[0].DiscreteValues = [Quantity('0[s]'),Quantity('1[s]'), \
    Quantity('2[s]'),Quantity('3[s]'),Quantity('4[s]')]
Tabular_Force.XComponent.Output.DiscreteValues = [Quantity('0[N]'),Quantity('0[N]'), \
    Quantity('5.e+005[N]'),Quantity('0[N]'),Quantity('-5.e+005[N]')]

Bolt_Pretension = STAT_STRUC.AddBoltPretension()
Bolt_Pretension.Location = shank_surface
Bolt_Pretension.Preload.Inputs[0].DiscreteValues = [Quantity('1[s]'),Quantity('2[s]'), \
    Quantity('3[s]'),Quantity('4[s]')]
Bolt_Pretension.Preload.Output.DiscreteValues = [Quantity('6.1363e+005[N]'), \
    Quantity('0 [N]'),Quantity('0 [N]'),Quantity('0[N]')]
Bolt_Pretension.SetDefineBy(2,BoltLoadDefineBy.Lock)
Bolt_Pretension.SetDefineBy(3,BoltLoadDefineBy.Lock)
Bolt_Pretension.SetDefineBy(4,BoltLoadDefineBy.Lock)

# Insert results.
Post_Contact_Tool = STAT_STRUC_SOLN.AddContactTool()
Post_Contact_Tool.ScopingMethod = GeometryDefineByType.Worksheet

Bolt_Tool = STAT_STRUC_SOLN.AddBoltTool()
Bolt_Working_Load = Bolt_Tool.AddWorkingLoad()

Total_Deformation = STAT_STRUC_SOLN.AddTotalDeformation()
Equivalent_stress_1 = STAT_STRUC_SOLN.AddEquivalentStress()
Equivalent_stress_2 = STAT_STRUC_SOLN.AddEquivalentStress()
Equivalent_stress_2.Location = shank
Force_Reaction_1 = STAT_STRUC_SOLN.AddForceReaction()
Force_Reaction_1.BoundaryConditionSelection = FIX_SUP
Moment_Reaction_2 = STAT_STRUC_SOLN.AddMomentReaction()
Moment_Reaction_2.BoundaryConditionSelection = FIX_SUP

# Set number of processors to 6 using DANSYS. (Optional)
# Num_Cores = STAT_STRUC.SolveConfiguration.SolveProcessSettings.MaxNumberOfCores
# STAT_STRUC.SolveConfiguration.SolveProcessSettings.MaxNumberOfCores = 6

# Solve and validate the results.
STAT_STRUC_SOLN.Solve(True)
STAT_STRUC_SS=STAT_STRUC_SOLN.Status

# Set the isometric view and zoom to fit.
cam = Graphics.Camera
cam.SetSpecificViewOrientation(ViewOrientationType.Iso)
cam.SetFit()

mechdir = STAT_STRUC.Children[0].SolverFilesDirectory
export_path = os.path.join(mechdir, "contact_status.png")
Post_Contact_Tool.Children[0].Activate()
Graphics.ExportImage(export_path, GraphicsImageExportFormat.PNG)

my_results_details = {
    "Total_Deformation": str(Total_Deformation.Maximum),
    "Equivalent_Stress1": str(Equivalent_stress_1.Maximum),
    "Equivalent_Stress2": str(Equivalent_stress_2.Maximum),
}

json.dumps(my_results_details)
"""
)
print(output)
{"Equivalent_Stress1": "1947.2385637831926 [MPa]", "Total_Deformation": "0.38462661294473227 [mm]", "Equivalent_Stress2": "1947.2385637831926 [MPa]"}

Initialize the variable needed for the image directory#

Set the image_dir variable for later use. Make the variable compatible for Windows, Linux, and Docker containers.

# image_directory_modified = project_directory.replace("\\", "\\\\")
mechanical.run_python_script(f"image_dir=ExtAPI.DataModel.AnalysisList[0].WorkingDir")


# Verify the path for image directory.
result_image_dir_server = mechanical.run_python_script(f"image_dir")
print(f"Images are stored on the server at: {result_image_dir_server}")
Images are stored on the server at: /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/

Download the image and plot#

Download one image file from the server to the current working directory and plot using matplotlib.

def get_image_path(image_name):
    return os.path.join(result_image_dir_server, image_name)


def display_image(path):
    print(f"Printing {path} using matplotlib")
    image1 = mpimg.imread(path)
    plt.figure(figsize=(15, 15))
    plt.axis("off")
    plt.imshow(image1)
    plt.show()


image_name = "contact_status.png"
image_path_server = get_image_path(image_name)

if image_path_server != "":
    current_working_directory = os.getcwd()

    local_file_path_list = mechanical.download(
        image_path_server, target_dir=current_working_directory
    )
    image_local_path = local_file_path_list[0]
    print(f"Local image path : {image_local_path}")

    display_image(image_local_path)
example 06 bolt pretension
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/contact_status.png to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/contact_status.png:   0%|          | 0.00/75.0k [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/contact_status.png to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/contact_status.png: 100%|██████████| 75.0k/75.0k [00:00<00:00, 362MB/s]
Local image path : /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/contact_status.png
Printing /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/contact_status.png using matplotlib

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):
    """Get the solve out path and return."""
    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):
    """Write file contents to console."""
    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()

    mechanical.download(solve_out_path, target_dir=current_working_directory)
    solve_out_local_path = os.path.join(current_working_directory, "solve.out")

    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/AnsysMechCE33/Project_Mech_Files/StaticStructural/solve.out to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/solve.out:   0%|          | 0.00/78.8k [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/solve.out to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/solve.out: 100%|██████████| 78.8k/78.8k [00:00<00:00, 383MB/s]

 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 2025 R1          LEGAL NOTICES          *
 ***************************************************************
 *                                                             *
 * Copyright 1971-2025 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).                                                  *
 *                                                             *
 ***************************************************************

 2025 R1

 Point Releases and Patches installed:

 Ansys, Inc. License Manager 2025 R1
 LS-DYNA 2025 R1
 Core WB Files 2025 R1
 Mechanical Products 2025 R1


          *****  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/AnsysMechCE33/Project_Mech_Files/StaticStructural/dummy.dat
  OUTPUT FILE NAME             = /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/solve.out
  START-UP FILE MODE           = NOREAD
  STOP FILE MODE               = NOREAD

 RELEASE= 2025 R1              BUILD= 25.1      UP20241202   VERSION=LINUX x64
 CURRENT JOBNAME=file0  06:58:57  APR 01, 2025 CP=      0.254


 PARAMETER _DS_PROGRESS =     999.0000000

 /INPUT FILE= ds.dat  LINE=       0



 *** NOTE ***                            CP =       0.355   TIME= 06:58:57
 The /CONFIG,NOELDB command is not valid in a distributed memory
 parallel solution.  Command is ignored.

 *GET  _WALLSTRT  FROM  ACTI  ITEM=TIME WALL  VALUE=  6.98250000

 TITLE=
 --Static Structural

  ACT Extensions:
      LSDYNA, 2025.1
      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/AnsysMechCE33/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/AnsysMechCE33/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/AnsysMechCE33/Project_Mech_Files/UserFiles/
 --- Data in consistent NMM units. See Solving Units in the help system for more

 MPA UNITS SPECIFIED FOR INTERNAL
  LENGTH      = MILLIMETERS (mm)
  MASS        = TONNE (Mg)
  TIME        = SECONDS (sec)
  TEMPERATURE = CELSIUS (C)
  TOFFSET     = 273.0
  FORCE       = NEWTON (N)
  HEAT        = MILLIJOULES (mJ)

 INPUT  UNITS ARE ALSO SET TO MPA

 *** MAPDL - ENGINEERING ANALYSIS SYSTEM  RELEASE 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:58:57  APR 01, 2025 CP=      0.359

 --Static Structural



          ***** MAPDL ANALYSIS DEFINITION (PREP7) *****
 *********** Nodes for the whole assembly ***********
 *********** Nodes for all Remote Points ***********
 *********** Elements for Body 1 'Solid' ***********
 *********** Elements for Body 3 'Solid' ***********
 *********** Elements for Body 5 'Solid' ***********
 *********** Elements for Body 7 'Solid' ***********
 *********** Elements for Body 9 'Solid' ***********
 *********** Elements for Body 11 'Solid' ***********
 *********** Send User Defined Coordinate System(s) ***********
 *********** Set Reference Temperature ***********
 *********** Send Materials ***********
 *********** Create Contact "Contact Region" ***********
             Real Constant Set For Above Contact Is 13 & 12
 *********** Create Contact "Contact Region 2" ***********
             Real Constant Set For Above Contact Is 15 & 14
 *********** Create Contact "Contact Region 3" ***********
             Real Constant Set For Above Contact Is 17 & 16
 *********** Create Contact "Contact Region 4" ***********
             Real Constant Set For Above Contact Is 19 & 18
 *********** Create Contact "Contact Region 5" ***********
             Real Constant Set For Above Contact Is 21 & 20
 *********** Create Contact "Contact Region 6" ***********
             Real Constant Set For Above Contact Is 23 & 22
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Element Component ***********
 *********** Send Named Selection as Element Component ***********
 *********** Send Named Selection as Element Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Send Named Selection as Node Component ***********
 *********** Fixed Supports ***********
 *********** Define Force Using Surface Effect Elements ***********
 *********** Create Bolt Pretension "Bolt Pretension" ***********
  CREATE COMPONENT CMEBOLT  FROM PRETENSION ELEMENTS
  CREATE COMPONENT CMNBOLT  FROM PRETENSION NODES


 ***** ROUTINE COMPLETED *****  CP =         1.055


 --- Number of total nodes = 20315
 --- Number of contact elements = 4628
 --- Number of spring elements = 0
 --- Number of bearing elements = 0
 --- Number of solid elements = 4404
 --- Number of condensed parts = 0
 --- Number of total elements = 9162

 *GET  _WALLBSOL  FROM  ACTI  ITEM=TIME WALL  VALUE=  6.98250000
 ****************************************************************************
 *************************    SOLUTION       ********************************
 ****************************************************************************

 *****  MAPDL SOLUTION ROUTINE  *****


 PERFORM A STATIC ANALYSIS
  THIS WILL BE A NEW ANALYSIS

 EQUATION PIVOT CHECKING LOGIC WILL BE DISABLED

 PRINT EQUATION PIVOT INFO ONCE PER LOADSTEP

 PARAMETER _THICKRATIO =    0.6670000000

 USE SPARSE MATRIX DIRECT SOLVER

 CONTACT INFORMATION PRINTOUT LEVEL       1

 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.

 DEFINE RESTART CONTROL FOR LOADSTEP LAST
 AT FREQUENCY OF LAST AND NUMBER FOR OVERWRITE IS   -1

 DELETE RESTART FILES OF ENDSTEP
 ****************************************************
 ******************* SOLVE FOR LS 1 OF 4 ****************

 SELECT       FOR ITEM=TYPE COMPONENT=
  IN RANGE        24 TO         24 STEP          1

         98  ELEMENTS (OF       9162  DEFINED) SELECTED BY  ESEL  COMMAND.

 SELECT      ALL NODES HAVING ANY ELEMENT IN ELEMENT SET.

        337 NODES (OF      20315  DEFINED) SELECTED FROM
       98 SELECTED ELEMENTS BY NSLE COMMAND.

 SPECIFIED SURFACE LOAD PRES FOR ALL SELECTED ELEMENTS  LKEY =  1   KVAL = 1
      SET ACCORDING TO TABLE PARAMETER = _LOADVARI153X

 SPECIFIED SURFACE LOAD PRES FOR ALL SELECTED ELEMENTS  LKEY =  2   KVAL = 1
     VALUES =     0.0000         0.0000         0.0000         0.0000

 SPECIFIED SURFACE LOAD PRES FOR ALL SELECTED ELEMENTS  LKEY =  3   KVAL = 1
     VALUES =     0.0000         0.0000         0.0000         0.0000

 ALL SELECT   FOR ITEM=NODE COMPONENT=
  IN RANGE         1 TO      20315 STEP          1

      20315  NODES (OF      20315  DEFINED) SELECTED BY NSEL  COMMAND.

 ALL SELECT   FOR ITEM=ELEM COMPONENT=
  IN RANGE         1 TO      11819 STEP          1

       9162  ELEMENTS (OF       9162  DEFINED) SELECTED BY  ESEL  COMMAND.

 PRINTOUT RESUMED BY /GOP

 SPECIFIED NODAL LOAD FX   FOR SELECTED NODES     20185 TO    20185 BY        1
  REAL=  613630.000       IMAG=  0.00000000

 DO NOT USE AUTOMATIC TIME STEPPING THIS LOAD STEP

 USE       2 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL  DEGREES OF FREEDOM
 FOR AUTOMATIC TIME STEPPING:
   USE      2 SUBSTEPS AS A MAXIMUM
   USE      2 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 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 =       1.143   TIME= 06:58:58
 The automatic domain decomposition logic has selected the MESH domain
 decomposition method with 4 processes per solution.

 *****  MAPDL SOLVE    COMMAND  *****

 *** WARNING ***                         CP =       1.180   TIME= 06:58:58
 Element shape checking is currently inactive.  Issue SHPP,ON or
 SHPP,WARN to reactivate, if desired.

 *** NOTE ***                            CP =       1.229   TIME= 06:58:58
 The model data was checked and warning messages were found.
  Please review output or errors file (
 /tmp/ANSYS.root.1/AnsysMechCE33/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 SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
 HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.

 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 SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
 HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.

 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

 ELEMENT TYPE         5 IS SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
 HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.

 ELEMENT TYPE         6 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         7 IS SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
 HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.

 ELEMENT TYPE         8 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         9 IS SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
 HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.

 ELEMENT TYPE        10 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        11 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 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:58:58  APR 01, 2025 CP=      1.239

 --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
   ANALYSIS TYPE . . . . . . . . . . . . . . . . .STATIC (STEADY-STATE)
   OFFSET TEMPERATURE FROM ABSOLUTE ZERO . . . . .  273.15
   EQUATION SOLVER OPTION. . . . . . . . . . . . .SPARSE
   NEWTON-RAPHSON OPTION . . . . . . . . . . . . .PROGRAM CHOSEN
   GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC

 *** WARNING ***                         CP =       1.282   TIME= 06:58:58
 Material number 24 (used by element 11592) should normally have at
 least one MP or one TB type command associated with it.  Output of
 energy by material may not be available.

 *** NOTE ***                            CP =       1.294   TIME= 06:58:58
 The step data was checked and warning messages were found.
  Please review output or errors file (
 /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/fil
 le0.err ) for these warning messages.

 *** NOTE ***                            CP =       1.295   TIME= 06:58:58
 This nonlinear analysis defaults to using the full Newton-Raphson
 solution procedure.  This can be modified using the NROPT command.
 *WARNING*: Some MPC/Lagrange based elements (e.g.7542) in real constant
 set 15 overlap with other MPC/Lagrange based elements (e.g.9536) in
 real constant set 21 which can cause overconstraint.

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 12 and contact element type 12 has been set up.  The
 companion pair has real constant set ID 13.  Both pairs should have
 the same behavior.
 *WARNING*: The contact pairs have similar mesh patterns which can cause
 overconstraint.  MAPDL will deactivate the current pair and keep its
 companion pair.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.18456E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance           1.3817
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000

 *** WARNING ***                         CP =       2.303   TIME= 06:58:58
 It is highly recommended to set KEYOPT(10)=0 (update contact stiffness
 at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.016
 Average contact pair depth                    13.817
 Average target surface length                 13.943
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  13.817
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 7162
 and target element 7368.
 ****************************************


 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 13 and contact element type 12 has been set up.  The
 companion pair has real constant set ID 12.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.18456E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance           1.4088
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000
 *WARNING*: It is highly recommended to set KEYOPT(10)=0 (update contact
 stiffness at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.007
 Average contact pair depth                    14.088
 Average target surface length                 13.942
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  14.088
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 7262
 and target element 7064.
 ****************************************


 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 14 and contact element type 14 has been set up.  The
 companion pair has real constant set ID 15.  Both pairs should have
 the same behavior.
 MAPDL will deactivate the current pair and keep its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 Average contact surface length                13.531
 Average contact pair depth                    9.0953
 Average target surface length                 6.3865
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  2.2738
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Max.  Initial penetration 0.684961413 was detected between contact
 element 7531 and target element 8553.
 You may move entire target surface by : x= 3.574949984E-16, y=
 -0.262123383, z= 0.632821831,to reduce initial penetration.
 ****************************************


 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 15 and contact element type 14 has been set up.  The
 companion pair has real constant set ID 14.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Distributed constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 *WARNING*: Certain contact elements (for example 8369&10363) overlap
 each other.  Overconstraint may occur.
 Average contact surface length                6.4480
 Average contact pair depth                    5.1166
 Average target surface length                 13.388
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  1.2792
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.303   TIME= 06:58:58
 Max.  Initial penetration 0.675803228 was detected between contact
 element 7817 and target element 7492.
 You may move entire target surface by : x= 3.618027317E-02, y=
 -0.234296751, z= -0.632855452,to reduce initial penetration.
 *WARNING*: The geometric gap/penetration may be too large.  Increase
 pinball radius if it is a true geometric gap/penetration.  Decrease
 pinball if it is a false one.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 16 and contact element type 16 has been set up.  The
 companion pair has real constant set ID 17.  Both pairs should have
 the same behavior.
 MAPDL will deactivate the current pair and keep its companion pair,
 resulting in asymmetric contact.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.21213E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance           1.2257
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000
 *WARNING*: It is highly recommended to set KEYOPT(10)=0 (update contact
 stiffness at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.017
 Average contact pair depth                    12.257
 Average target surface length                 14.211
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  12.257
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 9298
 and target element 9426.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 17 and contact element type 16 has been set up.  The
 companion pair has real constant set ID 16.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.21213E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance          0.44258
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000
 *WARNING*: It is highly recommended to set KEYOPT(10)=0 (update contact
 stiffness at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.576
 Average contact pair depth                    4.4258
 Average target surface length                 13.943
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  4.4258
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 9398
 and target element 9247.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 18 and contact element type 18 has been set up.  The
 companion pair has real constant set ID 19.  Both pairs should have
 the same behavior.
 MAPDL will deactivate the current pair and keep its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 Average contact surface length                14.393
 Average contact pair depth                    4.4329
 Average target surface length                 12.238
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  1.1082
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 5.684341886E-14 was detected between contact
 element 9446 and target element 9478.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 19 and contact element type 18 has been set up.  The
 companion pair has real constant set ID 18.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Distributed constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 *WARNING*: Certain contact elements (for example 9472&9524) overlap
 each other.  Overconstraint may occur.
 Average contact surface length                12.576
 Average contact pair depth                    12.199
 Average target surface length                 14.266
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  3.0498
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 8.526512829E-14 was detected between contact
 element 9459 and target element 9433.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 20 and contact element type 20 has been set up.  The
 companion pair has real constant set ID 21.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Distributed constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 *WARNING*: Certain contact elements (for example 9527&9464) overlap
 each other.  Overconstraint may occur.
 Average contact surface length                13.088
 Average contact pair depth                    6.7345
 Average target surface length                 6.3865
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  1.6836
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 1.28495889 was detected between contact
 element 9515 and target element 11105.
 You may move entire target surface by : x= 1.224539025E-15, y=
 -1.18655332, z= -0.493163843,to reduce initial penetration.
 *WARNING*: The geometric gap/penetration may be too large.  Increase
 pinball radius if it is a true geometric gap/penetration.  Decrease
 pinball if it is a false one.
 ****************************************


 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 21 and contact element type 20 has been set up.  The
 companion pair has real constant set ID 20.  Both pairs should have
 the same behavior.
 MAPDL will deactivate the current pair and keep its companion pair,
 resulting in asymmetric contact.
 Auto surface constraint is built
 Distributed constraint is built
 Contact algorithm: MPC based approach

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Contact related postprocess items (ETABLE, pressure ...) are not
 available.
 Contact detection at: nodal point (normal to target surface)
 MPC will be built internally to handle bonded contact.
 Average contact surface length                6.4480
 Average contact pair depth                    5.1166
 Average target surface length                 12.889
 Default pinball region factor PINB           0.25000
 The resulting pinball region                  1.2792
 Default target edge extension factor TOLS     2.0000
 Initial penetration/gap is excluded.
 Bonded contact (always) is defined.

 *** NOTE ***                            CP =       2.304   TIME= 06:58:58
 Max.  Initial penetration 1.2132628 was detected between contact
 element 10277 and target element 9491.
 You may move entire target surface by : x= 2.447930752E-02, y=
 1.1355368, z= 0.426571867,to reduce initial penetration.
 *WARNING*: The detected Max.  Penetration is close to the pair based
 pinball.  Please verify the pinball radius carefully.
 *WARNING*: The geometric gap/penetration may be too large.  Increase
 pinball radius if it is a true geometric gap/penetration.  Decrease
 pinball if it is a false one.
 ****************************************


 *** NOTE ***                            CP =       2.305   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 22 and contact element type 22 has been set up.  The
 companion pair has real constant set ID 23.  Both pairs should have
 the same behavior.
 *WARNING*: The contact pairs have similar mesh patterns which can cause
 overconstraint.  MAPDL will deactivate the current pair and keep its
 companion pair.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.18193E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance           1.4291
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000
 *WARNING*: It is highly recommended to set KEYOPT(10)=0 (update contact
 stiffness at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.016
 Average contact pair depth                    14.291
 Average target surface length                 13.943
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  14.291
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.305   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 11292
 and target element 11492.
 ****************************************


 *** NOTE ***                            CP =       2.305   TIME= 06:58:58
 Symmetric Deformable- deformable contact pair identified by real
 constant set 23 and contact element type 22 has been set up.  The
 companion pair has real constant set ID 22.  Both pairs should have
 the same behavior.
 MAPDL will keep the current pair and deactivate its companion pair,
 resulting in asymmetric contact.
 Contact algorithm: Augmented Lagrange method
 Contact detection at: Gauss integration point
 Contact stiffness factor FKN                  1.0000
 The resulting initial contact stiffness      0.18193E+06
 Default penetration tolerance factor FTOLN   0.10000
 The resulting penetration tolerance           1.2341
 Max. initial friction coefficient MU         0.20000
 Default tangent stiffness factor FKT          1.0000
 *WARNING*: It is highly recommended to set KEYOPT(10)=0 (update contact
 stiffness at each iteration) in order to achieve better convergence.
 Use constant contact stiffness
 Default Max. friction stress TAUMAX          0.10000E+21
 Average contact surface length                14.007
 Average contact pair depth                    12.341
 Average target surface length                 13.942
 Default pinball region factor PINB            1.0000
 The resulting pinball region                  12.341
 Contact offset is included. Initial geometric penetration is excluded.

 *** NOTE ***                            CP =       2.305   TIME= 06:58:58
 Max.  Initial penetration 0 was detected between contact element 11392
 and target element 11192.
 ****************************************


 *** WARNING ***                         CP =       2.305   TIME= 06:58:58
 Overconstraint may occur for Lagrange multiplier or MPC based contact
 algorithm.
 The reasons for possible overconstraint are:

 *** WARNING ***                         CP =       2.305   TIME= 06:58:58
 Certain contact elements (for example 9527 & 9464) overlap with other.
 ****************************************





     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: 9162
  ...Number of nodes:    20315
  ...Decompose to 4 CPU domains
  ...Element load balance ratio =     1.668


                      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. . . . . . . . . . . . . . .     2
   MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. . . .    15
   STEP CHANGE BOUNDARY CONDITIONS . . . . . . . .    NO
   TERMINATE ANALYSIS IF NOT CONVERGED . . . . . .YES (EXIT)
   CONVERGENCE CONTROLS. . . . . . . . . . . . . .USE DEFAULTS
   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
      CONT        ALL


 SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr

 >>>> PRETENSION ELEMENT STATUS <<<<
 SECTION NAME     PT.NODE  --------STATUS--------------------  ----LOAD SOURCE----
    25              20185  APPLIED PRELOAD FORCE= 0.61363E+06  F COMMAND
 MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS HAS BEEN MODIFIED
  TO BE, NEQIT = 26, BY SOLUTION CONTROL LOGIC.


 Range of element maximum matrix coefficients in global coordinates
 Maximum = 29991749.6 at element 2587.
 Minimum = 820595.982 at element 1132.

   *** ELEMENT MATRIX FORMULATION TIMES
     TYPE    NUMBER   ENAME      TOTAL CP  AVE CP

        1        80  SOLID187      0.005   0.000060
        2       976  SOLID186      0.114   0.000117
        3        79  SOLID187      0.005   0.000061
        4       985  SOLID186      0.116   0.000118
        5        14  SOLID187      0.001   0.000066
        6       445  SOLID186      0.053   0.000118
        7        10  SOLID187      0.001   0.000073
        8        51  SOLID186      0.007   0.000128
        9         4  SOLID187      0.000   0.000063
       10        58  SOLID186      0.008   0.000132
       11      1702  SOLID186      0.203   0.000119
       12       200  CONTA174      0.041   0.000206
       13       200  TARGE170      0.001   0.000004
       14       868  CONTA174      0.029   0.000034
       15       868  TARGE170      0.005   0.000006
       16       115  CONTA174      0.007   0.000063
       17       115  TARGE170      0.001   0.000004
       18        30  CONTA174      0.006   0.000190
       19        30  TARGE170      0.000   0.000005
       20       852  CONTA174      0.028   0.000033
       21       852  TARGE170      0.004   0.000005
       22       200  CONTA174      0.041   0.000204
       23       200  TARGE170      0.001   0.000005
       24        98  SURF154       0.004   0.000038
       25       130  PRETS179      0.000   0.000003
 Time at end of element matrix formulation CP = 3.92504311.

 ALL CURRENT MAPDL DATA WRITTEN TO FILE NAME= file.rdb
  FOR POSSIBLE RESUME FROM THIS POINT
     FORCE CONVERGENCE VALUE  =  0.3068E+06  CRITERION=   1534.

 DISTRIBUTED SPARSE MATRIX DIRECT SOLVER.
  Number of equations =       55204,    Maximum wavefront =    918


  Memory allocated on only this MPI rank (rank     0)
  -------------------------------------------------------------------
  Equation solver memory allocated                     =   138.310 MB
  Equation solver memory required for in-core mode     =   132.498 MB
  Equation solver memory required for out-of-core mode =    49.672 MB
  Total (solver and non-solver) memory allocated       =   852.935 MB


  Total memory summed across all MPI ranks on this machines
  -------------------------------------------------------------------
  Equation solver memory allocated                     =   495.936 MB
  Equation solver memory required for in-core mode     =   476.195 MB
  Equation solver memory required for out-of-core mode =   216.757 MB
  Total (solver and non-solver) memory allocated       =  2441.350 MB

 *** NOTE ***                            CP =       4.291   TIME= 06:58:59
 The Distributed Sparse Matrix Solver is currently running in the
 in-core memory mode.  This memory mode uses the most amount of memory
 in order to avoid using the hard drive as much as possible, which most
 often results in the fastest solution time.  This mode is recommended
 if enough physical memory is present to accommodate all of the solver
 data.
 curEqn=  14949  totEqn=  14949 Job CP sec=      4.525
      Factor Done= 100% Factor Wall sec=      0.320 rate=      27.1 GFlops
 Distributed sparse solver maximum pivot= 40670290.3 at node 1275 UX.
 Distributed sparse solver minimum pivot= 234121.19 at node 12641 UZ.
 Distributed sparse solver minimum pivot in absolute value= 234121.19 at
 node 12641 UZ.
     DISP CONVERGENCE VALUE   =  0.3397      CRITERION=  0.1699E-01
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.3397
     DISP CONVERGENCE VALUE   =  0.3397      CRITERION=  0.1699E-01
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.3397
     FORCE CONVERGENCE VALUE  =  0.2060E+05  CRITERION=   1544.
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.6354E-02
     DISP CONVERGENCE VALUE   =  0.6354E-02  CRITERION=  0.1721E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.6354E-02
     FORCE CONVERGENCE VALUE  =  0.1402E+05  CRITERION=   1543.
    EQUIL ITER   3 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.3153E-02
     DISP CONVERGENCE VALUE   =  0.3153E-02  CRITERION=  0.1734E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.3153E-02
     FORCE CONVERGENCE VALUE  =   5745.      CRITERION=   1542.
    EQUIL ITER   4 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1613E-02
     DISP CONVERGENCE VALUE   =  0.1613E-02  CRITERION=  0.1738E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC = -0.1613E-02
     FORCE CONVERGENCE VALUE  =   3511.      CRITERION=   1542.
    EQUIL ITER   5 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1301E-02
     DISP CONVERGENCE VALUE   =  0.1301E-02  CRITERION=  0.1740E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC = -0.1301E-02
     FORCE CONVERGENCE VALUE  =   3198.      CRITERION=   1542.
    EQUIL ITER   6 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.3924E-03
     DISP CONVERGENCE VALUE   =  0.3924E-03  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC = -0.3924E-03
     FORCE CONVERGENCE VALUE  =   724.5      CRITERION=   1542.     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   6

   *** ELEMENT RESULT CALCULATION TIMES
     TYPE    NUMBER   ENAME      TOTAL CP  AVE CP

        1        80  SOLID187      0.004   0.000053
        2       976  SOLID186      0.080   0.000082
        3        79  SOLID187      0.004   0.000056
        4       985  SOLID186      0.082   0.000084
        5        14  SOLID187      0.001   0.000056
        6       445  SOLID186      0.037   0.000084
        7        10  SOLID187      0.001   0.000061
        8        51  SOLID186      0.004   0.000084
        9         4  SOLID187      0.000   0.000062
       10        58  SOLID186      0.005   0.000094
       11      1702  SOLID186      0.145   0.000085
       12       200  CONTA174      0.012   0.000061
       14       868  CONTA174      0.023   0.000027
       16       115  CONTA174      0.004   0.000036
       18        30  CONTA174      0.001   0.000020
       20       852  CONTA174      0.016   0.000018
       22       200  CONTA174      0.012   0.000060
       24        98  SURF154       0.003   0.000026

   *** NODAL LOAD CALCULATION TIMES
     TYPE    NUMBER   ENAME      TOTAL CP  AVE CP

        1        80  SOLID187      0.001   0.000016
        2       976  SOLID186      0.016   0.000017
        3        79  SOLID187      0.001   0.000017
        4       985  SOLID186      0.017   0.000017
        5        14  SOLID187      0.000   0.000016
        6       445  SOLID186      0.008   0.000017
        7        10  SOLID187      0.000   0.000017
        8        51  SOLID186      0.001   0.000017
        9         4  SOLID187      0.000   0.000017
       10        58  SOLID186      0.001   0.000022
       11      1702  SOLID186      0.030   0.000018
       12       200  CONTA174      0.002   0.000009
       14       868  CONTA174      0.003   0.000003
       16       115  CONTA174      0.001   0.000006
       18        30  CONTA174      0.000   0.000003
       20       852  CONTA174      0.003   0.000003
       22       200  CONTA174      0.002   0.000008
       24        98  SURF154       0.000   0.000003
 *** LOAD STEP     1   SUBSTEP     1  COMPLETED.    CUM ITER =      6
 *** TIME =  0.500000         TIME INC =  0.500000

     FORCE CONVERGENCE VALUE  =   6376.      CRITERION=   3084.
     DISP CONVERGENCE VALUE   =  0.8045E-03  CRITERION=  0.1741E-01 <<< CONVERGED
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.8045E-03
     DISP CONVERGENCE VALUE   =  0.5598E-03  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.6958     SCALED MAX DOF INC = -0.5598E-03
     FORCE CONVERGENCE VALUE  =   1754.      CRITERION=   3084.     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   1
 *** LOAD STEP     1   SUBSTEP     2  COMPLETED.    CUM ITER =      7
 *** TIME =   1.00000         TIME INC =  0.500000


 *** MAPDL BINARY FILE STATISTICS
  BUFFER SIZE USED= 16384
        0.188 MB WRITTEN ON ELEMENT MATRIX FILE: file0.emat
        7.188 MB WRITTEN ON ELEMENT SAVED DATA FILE: file0.esav
       12.438 MB WRITTEN ON ASSEMBLED MATRIX FILE: file0.full
        2.625 MB WRITTEN ON RESULTS FILE: file0.rst
 *************** Write FE CONNECTORS *********

 WRITE OUT CONSTRAINT EQUATIONS TO FILE= file.ce
 ****************************************************
 *************** FINISHED SOLVE FOR LS 1 *************
 ****************************************************
 ******************* SOLVE FOR LS 2 OF 4 ****************

 PRINTOUT RESUMED BY /GOP

 DELETE ALL SPECIFIED NODAL LOADS FROM NODE     20185 TO     20185 BY       1

 NUMBER OF NODAL LOADS DELETED=       1

 *** WARNING ***                         CP =      11.990   TIME= 06:59:07
 Table _FIX is an MAPDL reserved table name.  It is used to constrain
 structural degrees of freedom to their current displaced status.  This
 table should not be used for other purposes.

 SPECIFIED CONSTRAINT UX   FOR SELECTED NODES        20185 TO       20185 BY           1
 SET ACCORDING TO TABLE PARAMETER = _FIX

 USE AUTOMATIC TIME STEPPING THIS LOAD STEP

 USE       1 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL  DEGREES OF FREEDOM
 FOR AUTOMATIC TIME STEPPING:
   USE     10 SUBSTEPS AS A MAXIMUM
   USE      1 SUBSTEPS AS A MINIMUM

 TIME=  2.0000

 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 CONT ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
   FOR ALL APPLICABLE ENTITIES

 *****  MAPDL SOLVE    COMMAND  *****

 *** WARNING ***                         CP =      12.101   TIME= 06:59:07
 Material number 24 (used by element 11592) should normally have at
 least one MP or one TB type command associated with it.  Output of
 energy by material may not be available.

 *** NOTE ***                            CP =      12.111   TIME= 06:59:07
 The step data was checked and warning messages were found.
  Please review output or errors file (
 /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/fil
 le0.err ) for these warning messages.

 *** NOTE ***                            CP =      12.112   TIME= 06:59:07
 This nonlinear analysis defaults to using the full Newton-Raphson
 solution procedure.  This can be modified using the NROPT command.

 *** MAPDL - ENGINEERING ANALYSIS SYSTEM  RELEASE 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:59:07  APR 01, 2025 CP=     12.321

 --Static Structural



                      L O A D   S T E P   O P T I O N S

   LOAD STEP NUMBER. . . . . . . . . . . . . . . .     2
   TIME AT END OF THE LOAD STEP. . . . . . . . . .  2.0000
   AUTOMATIC TIME STEPPING . . . . . . . . . . . .    ON
      INITIAL NUMBER OF SUBSTEPS . . . . . . . . .     1
      MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . .    10
      MINIMUM NUMBER OF SUBSTEPS . . . . . . . . .     1
   MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. . . .    15
   STEP CHANGE BOUNDARY CONDITIONS . . . . . . . .    NO
   TERMINATE ANALYSIS IF NOT CONVERGED . . . . . .YES (EXIT)
   CONVERGENCE CONTROLS. . . . . . . . . . . . . .USE DEFAULTS
   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
      CONT        ALL


 SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr

 >>>> PRETENSION ELEMENT STATUS <<<<
 SECTION NAME     PT.NODE  --------STATUS--------------------  ----LOAD SOURCE----
    25              20185  FIXED RELATIVE MOTION= 0.69601      D COMMAND
 MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS HAS BEEN MODIFIED
  TO BE, NEQIT = 26, BY SOLUTION CONTROL LOGIC.

     FORCE CONVERGENCE VALUE  =  0.4900E+05  CRITERION=   3094.
     DISP CONVERGENCE VALUE   =  0.1807E-01  CRITERION=  0.1741E-01
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.1807E-01
     DISP CONVERGENCE VALUE   =  0.1798E-01  CRITERION=  0.1741E-01
     LINE SEARCH PARAMETER =  0.9947     SCALED MAX DOF INC =  0.1798E-01
     FORCE CONVERGENCE VALUE  =  0.3010E+05  CRITERION=   3121.
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.7670E-02
     DISP CONVERGENCE VALUE   =  0.7173E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9351     SCALED MAX DOF INC =  0.7173E-02
     FORCE CONVERGENCE VALUE  =  0.2484E+05  CRITERION=   3121.
    EQUIL ITER   3 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.9770E-02
     DISP CONVERGENCE VALUE   =  0.9530E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9754     SCALED MAX DOF INC =  0.9530E-02
     FORCE CONVERGENCE VALUE  =  0.2325E+05  CRITERION=   3127.
    EQUIL ITER   4 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.8206E-02
     DISP CONVERGENCE VALUE   =  0.8206E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.8206E-02
     FORCE CONVERGENCE VALUE  =  0.1745E+05  CRITERION=   3132.
    EQUIL ITER   5 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.2773E-02
     DISP CONVERGENCE VALUE   =  0.2661E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9597     SCALED MAX DOF INC =  0.2661E-02
     FORCE CONVERGENCE VALUE  =  0.1851E+05  CRITERION=   3135.
    EQUIL ITER   6 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.2296E-02
     DISP CONVERGENCE VALUE   =  0.2296E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.2296E-02
     FORCE CONVERGENCE VALUE  =   8553.      CRITERION=   3137.
    EQUIL ITER   7 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.2497E-02
     DISP CONVERGENCE VALUE   =  0.2497E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.2497E-02
     FORCE CONVERGENCE VALUE  =   5753.      CRITERION=   3690.
    EQUIL ITER   8 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.9117E-03
     DISP CONVERGENCE VALUE   =  0.9117E-03  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.9117E-03
     FORCE CONVERGENCE VALUE  =   1854.      CRITERION=   3766.     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   8
 *** LOAD STEP     2   SUBSTEP     1  COMPLETED.    CUM ITER =     15
 *** TIME =   2.00000         TIME INC =   1.00000
 ****************************************************
 *************** FINISHED SOLVE FOR LS 2 *************
 ****************************************************
 ******************* SOLVE FOR LS 3 OF 4 ****************

 PRINTOUT RESUMED BY /GOP

 DELETE ALL SPECIFIED NODAL LOADS FROM NODE     20185 TO     20185 BY       1

 NUMBER OF NODAL LOADS DELETED=       0

 SPECIFIED CONSTRAINT UX   FOR SELECTED NODES        20185 TO       20185 BY           1
 SET ACCORDING TO TABLE PARAMETER = _FIX

 USE AUTOMATIC TIME STEPPING THIS LOAD STEP

 USE       1 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL  DEGREES OF FREEDOM
 FOR AUTOMATIC TIME STEPPING:
   USE     10 SUBSTEPS AS A MAXIMUM
   USE      1 SUBSTEPS AS A MINIMUM

 TIME=  3.0000

 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 CONT ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
   FOR ALL APPLICABLE ENTITIES

 *****  MAPDL SOLVE    COMMAND  *****

 *** WARNING ***                         CP =      22.180   TIME= 06:59:16
 Material number 24 (used by element 11592) should normally have at
 least one MP or one TB type command associated with it.  Output of
 energy by material may not be available.

 *** NOTE ***                            CP =      22.190   TIME= 06:59:16
 The step data was checked and warning messages were found.
  Please review output or errors file (
 /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/fil
 le0.err ) for these warning messages.

 *** NOTE ***                            CP =      22.190   TIME= 06:59:16
 This nonlinear analysis defaults to using the full Newton-Raphson
 solution procedure.  This can be modified using the NROPT command.

 *** MAPDL - ENGINEERING ANALYSIS SYSTEM  RELEASE 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:59:16  APR 01, 2025 CP=     22.353

 --Static Structural



                      L O A D   S T E P   O P T I O N S

   LOAD STEP NUMBER. . . . . . . . . . . . . . . .     3
   TIME AT END OF THE LOAD STEP. . . . . . . . . .  3.0000
   AUTOMATIC TIME STEPPING . . . . . . . . . . . .    ON
      INITIAL NUMBER OF SUBSTEPS . . . . . . . . .     1
      MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . .    10
      MINIMUM NUMBER OF SUBSTEPS . . . . . . . . .     1
   MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. . . .    15
   STEP CHANGE BOUNDARY CONDITIONS . . . . . . . .    NO
   TERMINATE ANALYSIS IF NOT CONVERGED . . . . . .YES (EXIT)
   CONVERGENCE CONTROLS. . . . . . . . . . . . . .USE DEFAULTS
   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
      CONT        ALL


 SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr

 >>>> PRETENSION ELEMENT STATUS <<<<
 SECTION NAME     PT.NODE  --------STATUS--------------------  ----LOAD SOURCE----
    25              20185  FIXED RELATIVE MOTION= 0.69601      D COMMAND
 MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS HAS BEEN MODIFIED
  TO BE, NEQIT = 26, BY SOLUTION CONTROL LOGIC.

     FORCE CONVERGENCE VALUE  =  0.4901E+05  CRITERION=   3130.
     DISP CONVERGENCE VALUE   =  0.8366E-01  CRITERION=  0.1741E-01
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.8366E-01
     DISP CONVERGENCE VALUE   =  0.7798E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9322E-01 SCALED MAX DOF INC = -0.7798E-02
     FORCE CONVERGENCE VALUE  =  0.2872E+06  CRITERION=   3128.
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.4199E-01
     DISP CONVERGENCE VALUE   =  0.9194E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.2190     SCALED MAX DOF INC = -0.9194E-02
     FORCE CONVERGENCE VALUE  =  0.3232E+06  CRITERION=   3114.
    EQUIL ITER   3 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2300E-01
     DISP CONVERGENCE VALUE   =  0.6408E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.2786     SCALED MAX DOF INC = -0.6408E-02
     FORCE CONVERGENCE VALUE  =  0.2862E+06  CRITERION=   3104.
    EQUIL ITER   4 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1093E-01
     DISP CONVERGENCE VALUE   =  0.5657E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.5176     SCALED MAX DOF INC = -0.5657E-02
     FORCE CONVERGENCE VALUE  =  0.2004E+06  CRITERION=   3092.
    EQUIL ITER   5 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.3956E-02
     DISP CONVERGENCE VALUE   =  0.3779E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9551     SCALED MAX DOF INC = -0.3779E-02
     FORCE CONVERGENCE VALUE  =  0.2067E+05  CRITERION=   3080.
    EQUIL ITER   6 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.1627E-02
     DISP CONVERGENCE VALUE   =  0.1386E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.8520     SCALED MAX DOF INC =  0.1386E-02
     FORCE CONVERGENCE VALUE  =   5992.      CRITERION=   3078.
    EQUIL ITER   7 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.9144E-03
     DISP CONVERGENCE VALUE   =  0.6790E-03  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.7426     SCALED MAX DOF INC = -0.6790E-03
     FORCE CONVERGENCE VALUE  =   3466.      CRITERION=   3618.     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   7
 *** LOAD STEP     3   SUBSTEP     1  COMPLETED.    CUM ITER =     22
 *** TIME =   3.00000         TIME INC =   1.00000
 ****************************************************
 *************** FINISHED SOLVE FOR LS 3 *************
 ****************************************************
 ******************* SOLVE FOR LS 4 OF 4 ****************

 PRINTOUT RESUMED BY /GOP

 DELETE ALL SPECIFIED NODAL LOADS FROM NODE     20185 TO     20185 BY       1

 NUMBER OF NODAL LOADS DELETED=       0

 SPECIFIED CONSTRAINT UX   FOR SELECTED NODES        20185 TO       20185 BY           1
 SET ACCORDING TO TABLE PARAMETER = _FIX

 USE AUTOMATIC TIME STEPPING THIS LOAD STEP

 USE       1 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL  DEGREES OF FREEDOM
 FOR AUTOMATIC TIME STEPPING:
   USE     10 SUBSTEPS AS A MAXIMUM
   USE      1 SUBSTEPS AS A MINIMUM

 TIME=  4.0000

 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 CONT ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
   FOR ALL APPLICABLE ENTITIES

 *****  MAPDL SOLVE    COMMAND  *****

 *** WARNING ***                         CP =      33.361   TIME= 06:59:27
 Material number 24 (used by element 11592) should normally have at
 least one MP or one TB type command associated with it.  Output of
 energy by material may not be available.

 *** NOTE ***                            CP =      33.371   TIME= 06:59:27
 The step data was checked and warning messages were found.
  Please review output or errors file (
 /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural/fil
 le0.err ) for these warning messages.

 *** NOTE ***                            CP =      33.372   TIME= 06:59:27
 This nonlinear analysis defaults to using the full Newton-Raphson
 solution procedure.  This can be modified using the NROPT command.

 *** MAPDL - ENGINEERING ANALYSIS SYSTEM  RELEASE 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:59:27  APR 01, 2025 CP=     33.548

 --Static Structural



                      L O A D   S T E P   O P T I O N S

   LOAD STEP NUMBER. . . . . . . . . . . . . . . .     4
   TIME AT END OF THE LOAD STEP. . . . . . . . . .  4.0000
   AUTOMATIC TIME STEPPING . . . . . . . . . . . .    ON
      INITIAL NUMBER OF SUBSTEPS . . . . . . . . .     1
      MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . .    10
      MINIMUM NUMBER OF SUBSTEPS . . . . . . . . .     1
   MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. . . .    15
   STEP CHANGE BOUNDARY CONDITIONS . . . . . . . .    NO
   TERMINATE ANALYSIS IF NOT CONVERGED . . . . . .YES (EXIT)
   CONVERGENCE CONTROLS. . . . . . . . . . . . . .USE DEFAULTS
   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
      CONT        ALL


 SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr

 >>>> PRETENSION ELEMENT STATUS <<<<
 SECTION NAME     PT.NODE  --------STATUS--------------------  ----LOAD SOURCE----
    25              20185  FIXED RELATIVE MOTION= 0.69601      D COMMAND
 MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS HAS BEEN MODIFIED
  TO BE, NEQIT = 26, BY SOLUTION CONTROL LOGIC.

     FORCE CONVERGENCE VALUE  =  0.4911E+05  CRITERION=   3088.
     DISP CONVERGENCE VALUE   =  0.1818E-01  CRITERION=  0.1741E-01
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1818E-01
     DISP CONVERGENCE VALUE   =  0.1785E-01  CRITERION=  0.1741E-01
     LINE SEARCH PARAMETER =  0.9817     SCALED MAX DOF INC = -0.1785E-01
     FORCE CONVERGENCE VALUE  =  0.1005E+05  CRITERION=   3067.
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.2206E-02
     DISP CONVERGENCE VALUE   =  0.2016E-02  CRITERION=  0.1741E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.9137     SCALED MAX DOF INC =  0.2016E-02
     FORCE CONVERGENCE VALUE  =   2958.      CRITERION=   3069.     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   2
 *** LOAD STEP     4   SUBSTEP     1  COMPLETED.    CUM ITER =     24
 *** TIME =   4.00000         TIME INC =   1.00000
 ****************************************************
 *************** FINISHED SOLVE FOR LS 4 *************

 *GET  _WALLASOL  FROM  ACTI  ITEM=TIME WALL  VALUE=  6.99166667

 PRINTOUT RESUMED BY /GOP

 FINISH SOLUTION PROCESSING


 ***** ROUTINE COMPLETED *****  CP =        37.196



 *** MAPDL - ENGINEERING ANALYSIS SYSTEM  RELEASE 2025 R1          25.1     ***
 Ansys Mechanical Enterprise
 00000000  VERSION=LINUX x64     06:59:30  APR 01, 2025 CP=     37.205

 --Static Structural



          ***** MAPDL RESULTS INTERPRETATION (POST1) *****

 *** NOTE ***                            CP =      37.205   TIME= 06:59:30
 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 =        37.209



 PRINTOUT RESUMED BY /GOP

 *GET  _WALLDONE  FROM  ACTI  ITEM=TIME WALL  VALUE=  6.99166667

 PARAMETER _PREPTIME =     0.000000000

 PARAMETER _SOLVTIME =     33.00000000

 PARAMETER _POSTTIME =     0.000000000

 PARAMETER _TOTALTIM =     33.00000000

 *GET  _DLBRATIO  FROM  ACTI  ITEM=SOLU DLBR  VALUE=  1.66797753

 *GET  _COMBTIME  FROM  ACTI  ITEM=SOLU COMB  VALUE= 0.750589747E-01

 *GET  _SSMODE   FROM  ACTI  ITEM=SOLU SSMM  VALUE=  2.00000000

 *GET  _NDOFS    FROM  ACTI  ITEM=SOLU NDOF  VALUE=  55203.0000

 *GET  _SOL_END_TIME  FROM  ACTI  ITEM=SET  TIME  VALUE=  4.00000000

 *IF  _sol_end_time  ( =   4.00000     )  EQ
      4.000000  ( =   4.00000     )  THEN

 /FCLEAN COMMAND REMOVING ALL LOCAL FILES

 *ENDIF
 --- Total number of nodes = 20315
 --- Total number of elements = 9162
 --- Element load balance ratio = 1.66797753
 --- Time to combine distributed files = 7.505897474E-02
 --- Sparse memory mode = 2
 --- Number of DOF = 55203

 EXIT MAPDL WITHOUT SAVING DATABASE


 NUMBER OF WARNING MESSAGES ENCOUNTERED=          9
 NUMBER OF ERROR   MESSAGES ENCOUNTERED=          0

+--------------------- M A P D L   S T A T I S T I C S ------------------------+

Release: 2025 R1            Build: 25.1       Update: UP20241202   Platform: LINUX x64
Date Run: 04/01/2025   Time: 06:59     Process ID: 3983
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: OPENMPI
MPI Version: Open MPI v4.0.5

GPU Acceleration: Not Requested

Job Name: file0
Input File: dummy.dat

  Core                Machine Name   Working Directory
 -----------------------------------------------------
     0                e3019d8c190a   /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural
     1                e3019d8c190a   /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural
     2                e3019d8c190a   /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural
     3                e3019d8c190a   /tmp/ANSYS.root.1/AnsysMechCE33/Project_Mech_Files/StaticStructural

Latency time from master to core     1 =    2.283 microseconds
Latency time from master to core     2 =    2.429 microseconds
Latency time from master to core     3 =    2.286 microseconds

Communication speed from master to core     1 = 16026.86 MB/sec
Communication speed from master to core     2 = 18346.81 MB/sec
Communication speed from master to core     3 = 16613.78 MB/sec

Total CPU time for main thread                    :       32.3 seconds
Total CPU time summed for all threads             :       37.4 seconds

Elapsed time spent obtaining a license            :        0.4 seconds
Elapsed time spent pre-processing model (/PREP7)  :        0.2 seconds
Elapsed time spent solution - preprocessing       :        0.8 seconds
Elapsed time spent computing solution             :       30.9 seconds
Elapsed time spent solution - postprocessing      :        0.1 seconds
Elapsed time spent post-processing model (/POST1) :        0.0 seconds

Equation solver used                              :            Sparse (symmetric)
Equation solver computational rate                :      100.8 Gflops
Equation solver effective I/O rate                :      125.1 GB/sec

Sum of disk space used on all processes           :      189.9 MB

Sum of memory used on all processes               :      752.0 MB
Sum of memory allocated on all processes          :     3228.0 MB
Physical memory available                         :         31 GB
Total amount of I/O written to disk               :        2.1 GB
Total amount of I/O read from disk                :       11.0 GB

+------------------ E N D   M A P D L   S T A T I S T I C S -------------------+


 *-----------------------------------------------------------------------------*
 |                                                                             |
 |                               RUN COMPLETED                                 |
 |                                                                             |
 |-----------------------------------------------------------------------------|
 |                                                                             |
 |  Ansys MAPDL 2025 R1         Build 25.1         UP20241202    LINUX x64     |
 |                                                                             |
 |-----------------------------------------------------------------------------|
 |                                                                             |
 |  Database Requested(-db)     1024 MB     Scratch Memory Requested   1024 MB |
 |  Max Database Used(Master)     20 MB     Max Scratch Used(Master)    191 MB |
 |  Max Database Used(Workers)     1 MB     Max Scratch Used(Workers)   193 MB |
 |  Sum Database Used(All)        23 MB     Sum Scratch Used(All)       729 MB |
 |                                                                             |
 |-----------------------------------------------------------------------------|
 |                                                                             |
 |        CP Time      (sec) =         37.373       Time  =  06:59:30          |
 |        Elapsed Time (sec) =         34.000       Date  =  04/01/2025        |
 |                                                                             |
 *-----------------------------------------------------------------------------*

Close mechanical#

Close the mechanical instance.

mechanical.exit()

Total running time of the script: (0 minutes 50.147 seconds)

Gallery generated by Sphinx-Gallery