Note
Go to the end to download the full example code.
Basic valve implementation#
This example demonstrates a basic implementation of a valve in Python.
Import the necessary libraries#
from pathlib import Path
from typing import TYPE_CHECKING
from matplotlib import image as mpimg, pyplot as plt
from matplotlib.animation import FuncAnimation
from PIL import Image
from ansys.mechanical.core import App
from ansys.mechanical.core.examples import delete_downloads, download_file
if TYPE_CHECKING:
import Ansys
Initialize the embedded application#
app = App(globals=globals())
print(app)
Ansys Mechanical [Ansys Mechanical Enterprise]
Product Version:261
Software build date: 01/12/2026 14:14:35
Create functions to set camera and display images#
# Set the path for the output files (images, gifs, mechdat)
output_path = Path.cwd() / "out"
def set_camera_and_display_image(
camera,
graphics,
graphics_image_export_settings,
image_output_path: Path,
image_name: str,
) -> None:
"""Set the camera to fit the model and display the image.
Parameters
----------
camera : Ansys.ACT.Common.Graphics.MechanicalCameraWrapper
The camera object to set the view.
graphics : Ansys.ACT.Common.Graphics.MechanicalGraphicsWrapper
The graphics object to export the image.
graphics_image_export_settings : Ansys.Mechanical.Graphics.GraphicsImageExportSettings
The settings for exporting the image.
image_output_path : Path
The path to save the exported image.
image_name : str
The name of the exported image file.
"""
# Set the camera to fit the mesh
camera.SetFit()
# Export the mesh image with the specified settings
image_path = image_output_path / image_name
graphics.ExportImage(str(image_path), image_export_format, graphics_image_export_settings)
# Display the exported mesh image
display_image(image_path)
def display_image(
image_path: str,
pyplot_figsize_coordinates: tuple = (16, 9),
plot_xticks: list = [],
plot_yticks: list = [],
plot_axis: str = "off",
) -> None:
"""Display the image with the specified parameters.
Parameters
----------
image_path : str
The path to the image file to display.
pyplot_figsize_coordinates : tuple
The size of the figure in inches (width, height).
plot_xticks : list
The x-ticks to display on the plot.
plot_yticks : list
The y-ticks to display on the plot.
plot_axis : str
The axis visibility setting ('on' or 'off').
"""
# Set the figure size based on the coordinates specified
plt.figure(figsize=pyplot_figsize_coordinates)
# Read the image from the file into an array
plt.imshow(mpimg.imread(image_path))
# Get or set the current tick locations and labels of the x-axis
plt.xticks(plot_xticks)
# Get or set the current tick locations and labels of the y-axis
plt.yticks(plot_yticks)
# Turn off the axis
plt.axis(plot_axis)
# Display the figure
plt.show()
Configure graphics for image export#
graphics = app.Graphics
camera = graphics.Camera
# Set the camera orientation to the isometric view
camera.SetSpecificViewOrientation(ViewOrientationType.Iso)
# Set the image export format and settings
image_export_format = GraphicsImageExportFormat.PNG
settings_720p = Ansys.Mechanical.Graphics.GraphicsImageExportSettings()
settings_720p.Resolution = GraphicsResolutionType.EnhancedResolution
settings_720p.Background = GraphicsBackgroundType.White
settings_720p.Width = 1280
settings_720p.Height = 720
settings_720p.CurrentGraphicsDisplay = False
Download and import the geometry file#
# Download the geometry file
geometry_path = download_file("Valve.pmdb", "pymechanical", "embedding")
Import the geometry
# Define the model
model = app.Model
# Add a geometry import to the geometry import group
geometry_import = model.GeometryImportGroup.AddGeometryImport()
# Set the geometry import settings
geometry_import_format = Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.Format.Automatic
geometry_import_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
geometry_import_preferences.ProcessNamedSelections = True
# Import the geometry file with the specified settings
geometry_import.Import(geometry_path, geometry_import_format, geometry_import_preferences)
# Visualize the model in 3D
app.plot()
[]
Assign the materials and mesh the geometry#
# Add the material assignment to the model materials
material_assignment = model.Materials.AddMaterialAssignment()
# Set the material to structural steel
material_assignment.Material = "Structural Steel"
# Create selection information for the geometry entities
selection_info = app.ExtAPI.SelectionManager.CreateSelectionInfo(
Ansys.ACT.Interfaces.Common.SelectionTypeEnum.GeometryEntities
)
# Get the geometric bodies from the model and add their IDs to the selection info IDs list
selection_info.Ids = [
body.GetGeoBody().Id
for body in model.Geometry.GetChildren(
Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Body, True
)
]
# Set the material assignment location to the selected geometry entities
material_assignment.Location = selection_info
Define the mesh settings and generate the mesh
# Define the mesh
mesh = model.Mesh
# Set the mesh element size to 25mm
mesh.ElementSize = Quantity(25, "mm")
# Generate the mesh
mesh.GenerateMesh()
# Activate the mesh and display the image
app.Tree.Activate([mesh])
set_camera_and_display_image(camera, graphics, settings_720p, output_path, "mesh.png")
Add a static structural analysis and apply boundary conditions#
# Add a static structural analysis to the model
analysis = model.AddStaticStructuralAnalysis()
# Add a fixed support to the analysis
fixed_support = analysis.AddFixedSupport()
# Set the fixed support location to the "NSFixedSupportFaces" object
fixed_support.Location = app.ExtAPI.DataModel.GetObjectsByName("NSFixedSupportFaces")[0]
# Add a frictionless support to the analysis
frictionless_support = analysis.AddFrictionlessSupport()
# Set the frictionless support location to the "NSFrictionlessSupportFaces" object
frictionless_support.Location = app.ExtAPI.DataModel.GetObjectsByName("NSFrictionlessSupportFaces")[
0
]
# Add pressure to the analysis
pressure = analysis.AddPressure()
# Set the pressure location to the "NSInsideFaces" object
pressure.Location = app.ExtAPI.DataModel.GetObjectsByName("NSInsideFaces")[0]
# Set the pressure magnitude's input and output values
pressure.Magnitude.Inputs[0].DiscreteValues = [Quantity("0 [s]"), Quantity("1 [s]")]
pressure.Magnitude.Output.DiscreteValues = [Quantity("0 [Pa]"), Quantity("15 [MPa]")]
# Activate the analysis and display the image
analysis.Activate()
set_camera_and_display_image(
camera, graphics, settings_720p, output_path, "boundary_conditions.png"
)
Add results to the analysis solution
# Define the solution for the analysis
solution = analysis.Solution
# Add the total deformation and equivalent stress results to the solution
deformation = solution.AddTotalDeformation()
stress = solution.AddEquivalentStress()
Solve the solution#
solution.Solve(True)
Show messages#
# Print all messages from Mechanical
app.messages.show()
Severity: Warning
DisplayString: Some boundaries of protected topologies have been defeatured. Right click on this message and select "Show Problematic Geometry" to see the affected edges.
Severity: Info
DisplayString: The requested license was received from the License Manager after 34 seconds.
Display the results#
Show the total deformation image
# Activate the total deformation result and display the image
app.Tree.Activate([deformation])
set_camera_and_display_image(
camera, graphics, settings_720p, output_path, "total_deformation_valve.png"
)
Show the equivalent stress image
# Activate the equivalent stress result and display the image
app.Tree.Activate([stress])
set_camera_and_display_image(camera, graphics, settings_720p, output_path, "stress_valve.png")
Create a function to update the animation frames
def update_animation(frame: int) -> list[mpimg.AxesImage]:
"""Update the animation frame for the GIF.
Parameters
----------
frame : int
The frame number to update the animation.
Returns
-------
list[mpimg.AxesImage]
A list containing the updated image for the animation.
"""
# Seeks to the given frame in this sequence file
gif.seek(frame)
# Set the image array to the current frame of the GIF
image.set_data(gif.convert("RGBA"))
# Return the updated image
return [image]
Export the stress animation
# Set the animation export format and settings
animation_export_format = Ansys.Mechanical.DataModel.Enums.GraphicsAnimationExportFormat.GIF
settings_720p = Ansys.Mechanical.Graphics.AnimationExportSettings()
settings_720p.Width = 1280
settings_720p.Height = 720
# Export the animation of the equivalent stress result
valve_gif = output_path / "valve.gif"
stress.ExportAnimation(str(valve_gif), animation_export_format, settings_720p)
# Open the GIF file and create an animation
gif = Image.open(valve_gif)
# Set the subplots for the animation and turn off the axis
figure, axes = plt.subplots(figsize=(16, 9))
axes.axis("off")
# Change the color of the image
image = axes.imshow(gif.convert("RGBA"))
# Create the animation using the figure, update_animation function, and the GIF frames
# Set the interval between frames to 200 milliseconds and repeat the animation
FuncAnimation(
figure,
update_animation,
frames=range(gif.n_frames),
interval=100,
repeat=True,
blit=True,
)
# Show the animation
plt.show()
Display the output file from the solve#
# Get the path to the solve output file
solve_path = Path(analysis.WorkingDir)
# Get the solve output file path
solve_out_path = solve_path / "solve.out"
# If the solve output file exists, print its contents
if solve_out_path:
with solve_out_path.open("rt") as file:
for line in file:
print(line, end="")
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 2026 R1 LEGAL NOTICES *
***************************************************************
* *
* Copyright (c) 2026 Synopsys, Inc. and 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). *
* *
***************************************************************
2026 R1
Point Releases and Patches installed:
Ansys, Inc. License Manager 2026 R1
LS-DYNA 2026 R1
Core WB Files 2026 R1
Mechanical Products 2026 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 = /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/dummy.dat
OUTPUT FILE NAME = /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/solve.out
START-UP FILE MODE = NOREAD
STOP FILE MODE = NOREAD
RELEASE= 2026 R1 BUILD= 26.1 UP20260112 VERSION=LINUX x64
CURRENT JOBNAME=file0 22:15:43 JAN 27, 2026 Elapsed Time= 0.238
PARAMETER _DS_PROGRESS = 999.0000000
/INPUT FILE= ds.dat LINE= 0
*** NOTE *** ELAPSED TIME = 0.601 TIME= 22:15:43
The /CONFIG,NOELDB command is not valid in a distributed memory
parallel solution. Command is ignored.
*GET _WALLSTRT FROM ACTI ITEM=TIME WALL VALUE= 0.167634453E-03
TITLE=
--Static Structural
SET PARAMETER DIMENSIONS ON _WB_PROJECTSCRATCH_DIR
TYPE=STRI DIMENSIONS= 248 1 1
PARAMETER _WB_PROJECTSCRATCH_DIR(1) = /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/
SET PARAMETER DIMENSIONS ON _WB_SOLVERFILES_DIR
TYPE=STRI DIMENSIONS= 248 1 1
PARAMETER _WB_SOLVERFILES_DIR(1) = /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/
SET PARAMETER DIMENSIONS ON _WB_USERFILES_DIR
TYPE=STRI DIMENSIONS= 248 1 1
PARAMETER _WB_USERFILES_DIR(1) = /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/UserFiles/
--- Data in consistent MKS units. See Solving Units in the help system for more
MKS UNITS SPECIFIED FOR INTERNAL
LENGTH (l) = METER (M)
MASS (M) = KILOGRAM (KG)
TIME (t) = SECOND (SEC)
TEMPERATURE (T) = CELSIUS (C)
TOFFSET = 273.0
CHARGE (Q) = COULOMB
FORCE (f) = NEWTON (N) (KG-M/SEC2)
HEAT = JOULE (N-M)
PRESSURE = PASCAL (NEWTON/M**2)
ENERGY (W) = JOULE (N-M)
POWER (P) = WATT (N-M/SEC)
CURRENT (i) = AMPERE (COULOMBS/SEC)
CAPACITANCE (C) = FARAD
INDUCTANCE (L) = HENRY
MAGNETIC FLUX = WEBER
RESISTANCE (R) = OHM
ELECTRIC POTENTIAL = VOLT
INPUT UNITS ARE ALSO SET TO MKS
*** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2026 R1 26.1 ***
Ansys Mechanical Enterprise
00000000 VERSION=LINUX x64 22:15:43 JAN 27, 2026 Elapsed Time= 0.604
--Static Structural
***** MAPDL ANALYSIS DEFINITION (PREP7) *****
*********** Send User Defined Coordinate System(s) ***********
*********** Nodes for the whole assembly ***********
*********** Elements for Body 1 'Connector\Solid1' ***********
*********** Elements for Body 2 'Right_elbow\Solid1' ***********
*********** Elements for Body 3 'Left_elbow\Solid1' ***********
*********** Set Reference Temperature ***********
*********** Send Materials ***********
*********** Create Contact "Contact Region" ***********
Real Constant Set For Above Contact Is 5 & 4
*********** Create Contact "Contact Region 2" ***********
Real Constant Set For Above Contact Is 7 & 6
*********** Send Named Selection as Node Component ***********
*********** Send Named Selection as Node Component ***********
*********** Send Named Selection as Node Component ***********
*********** Fixed Supports ***********
********* Frictionless Supports X *********
********* Frictionless Supports Z *********
*********** Node Rotations ***********
*********** Define Pressure Using Surface Effect Elements "Pressure" **********
***** ROUTINE COMPLETED ***** ELAPSED TIME = 0.859
--- Number of total nodes = 75886
--- Number of contact elements = 4698
--- Number of spring elements = 0
--- Number of bearing elements = 0
--- Number of solid elements = 47698
--- Number of condensed parts = 0
--- Number of total elements = 52396
*GET _WALLBSOL FROM ACTI ITEM=TIME WALL VALUE= 0.240223712E-03
****************************************************************************
************************* SOLUTION ********************************
****************************************************************************
***** MAPDL SOLUTION ROUTINE *****
PERFORM A STATIC ANALYSIS
THIS WILL BE A NEW ANALYSIS
PARAMETER _THICKRATIO = 0.3330000000
USE SPARSE MATRIX DIRECT SOLVER
CONTACT INFORMATION PRINTOUT LEVEL 1
CHECK INITIAL OPEN/CLOSED STATUS OF SELECTED CONTACT ELEMENTS
AND LIST DETAILED CONTACT PAIR INFORMATION
SPLIT CONTACT SURFACES AT SOLVE PHASE
NUMBER OF SPLITTING TBD BY PROGRAM
DO NOT COMBINE ELEMENT MATRIX FILES (.emat) AFTER DISTRIBUTED PARALLEL SOLUTION
DO NOT COMBINE ELEMENT SAVE DATA FILES (.esav) AFTER DISTRIBUTED PARALLEL SOLUTION
NLDIAG: Nonlinear diagnostics CONT option is set to ON.
Writing frequency : each ITERATION.
DO NOT SAVE ANY RESTART FILES AT ALL
****************************************************
******************* SOLVE FOR LS 1 OF 1 ****************
SELECT FOR ITEM=TYPE COMPONENT=
IN RANGE 8 TO 8 STEP 1
1664 ELEMENTS (OF 52396 DEFINED) SELECTED BY ESEL COMMAND.
SELECT ALL NODES HAVING ANY ELEMENT IN ELEMENT SET.
3460 NODES (OF 75886 DEFINED) SELECTED FROM
1664 SELECTED ELEMENTS BY NSLE COMMAND.
GENERATE SURFACE LOAD PRES ON SURFACE DEFINED BY ALL SELECTED NODES
SET ACCORDING TO TABLE PARAMETER = _LOADVARI56
NUMBER OF PRES ELEMENT FACE LOADS STORED = 1664
ALL SELECT FOR ITEM=NODE COMPONENT=
IN RANGE 1 TO 75886 STEP 1
75886 NODES (OF 75886 DEFINED) SELECTED BY NSEL COMMAND.
ALL SELECT FOR ITEM=ELEM COMPONENT=
IN RANGE 1 TO 64302 STEP 1
52396 ELEMENTS (OF 52396 DEFINED) SELECTED BY ESEL COMMAND.
ALL SELECT FOR ITEM=ELEM COMPONENT=
IN RANGE 1 TO 64302 STEP 1
52396 ELEMENTS (OF 52396 DEFINED) SELECTED BY ESEL COMMAND.
PRINTOUT RESUMED BY /GOP
USE 1 SUBSTEPS INITIALLY THIS LOAD STEP FOR ALL DEGREES OF FREEDOM
FOR AUTOMATIC TIME STEPPING:
USE 1 SUBSTEPS AS A MAXIMUM
USE 1 SUBSTEPS AS A MINIMUM
TIME= 1.0000
ERASE THE CURRENT DATABASE OUTPUT CONTROL TABLE.
WRITE ALL ITEMS TO THE DATABASE WITH A FREQUENCY OF NONE
FOR ALL APPLICABLE ENTITIES
WRITE NSOL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE RSOL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE EANG ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE ETMP ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE VENG ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE STRS ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE EPEL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE EPPL ITEMS TO THE DATABASE WITH A FREQUENCY OF ALL
FOR ALL APPLICABLE ENTITIES
WRITE 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 *** ELAPSED TIME = 0.951 TIME= 22:15:43
The automatic domain decomposition logic has selected the MESH domain
decomposition method with 4 processes per solution.
***** MAPDL SOLVE COMMAND *****
*** WARNING *** ELAPSED TIME = 1.009 TIME= 22:15:43
Element shape checking is currently inactive. Issue SHPP,ON or
SHPP,WARN to reactivate, if desired.
*** NOTE *** ELAPSED TIME = 1.068 TIME= 22:15:43
The model data was checked and warning messages were found.
Please review output or errors file ( /github/home/.mw/Application
Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/file0
0.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 SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.
ELEMENT TYPE 3 IS SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE AND NO RESETTING IS NEEDED.
*** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2026 R1 26.1 ***
Ansys Mechanical Enterprise
00000000 VERSION=LINUX x64 22:15:43 JAN 27, 2026 Elapsed Time= 1.077
--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
GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC
*** WARNING *** ELAPSED TIME = 1.104 TIME= 22:15:43
Material number 8 (used by element 62639) 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 *** ELAPSED TIME = 1.112 TIME= 22:15:43
The step data was checked and warning messages were found.
Please review output or errors file ( /github/home/.mw/Application
Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural/file0
0.err ) for these warning messages.
*** NOTE *** ELAPSED TIME = 1.112 TIME= 22:15:43
The conditions for direct assembly have been met. No .emat or .erot
files will be produced.
TRIM CONTACT/TARGET SURFACE
START TRIMMING SMALL/BONDED CONTACT PAIRS FOR DMP RUN.
741 CONTACT ELEMENTS & 776 TARGET ELEMENTS ARE DELETED DUE TO TRIMMING LOGIC.
2 CONTACT PAIRS ARE REMOVED.
CHECK INITIAL OPEN/CLOSED STATUS OF SELECTED CONTACT ELEMENTS
AND LIST DETAILED CONTACT PAIR INFORMATION
*** NOTE *** ELAPSED TIME = 1.690 TIME= 22:15:44
The maximum number of contact elements in any single contact pair is
396, which is smaller than the optimal domain size of 3029 elements
for the given number of CPU domains (4). Therefore, no contact pairs
are being split by the CNCH,DMP logic.
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
Deformable-deformable contact pair identified by real constant set 4
and contact element type 4 has been set up.
Auto surface constraint is built
Contact algorithm: MPC based approach
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
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 0.96911E-02
Average contact pair depth 0.61248E-02
Average target surface length 0.99228E-02
Default pinball region factor PINB 0.25000
The resulting pinball region 0.15312E-02
Default target edge extension factor TOLS 2.0000
Initial penetration/gap is excluded.
Bonded contact (always) is defined.
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
Max. Initial penetration 8.326672685E-17 was detected between contact
element 60043 and target element 61062.
****************************************
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
Deformable-deformable contact pair identified by real constant set 7
and contact element type 6 has been set up.
Auto surface constraint is built
Contact algorithm: MPC based approach
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
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 0.99792E-02
Average contact pair depth 0.59035E-02
Average target surface length 0.97921E-02
Default pinball region factor PINB 0.25000
The resulting pinball region 0.14759E-02
Default target edge extension factor TOLS 2.0000
Initial penetration/gap is excluded.
Bonded contact (always) is defined.
*** NOTE *** ELAPSED TIME = 1.931 TIME= 22:15:44
Max. Initial penetration 9.153579117E-17 was detected between contact
element 61983 and target element 61240.
****************************************
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: 50879
...Number of nodes: 75886
...Decompose to 4 CPU domains
...Element load balance ratio = 1.012
L O A D S T E P O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . . . . 1
TIME AT END OF THE LOAD STEP. . . . . . . . . . 1.0000
NUMBER OF SUBSTEPS. . . . . . . . . . . . . . . 1
STEP CHANGE BOUNDARY CONDITIONS . . . . . . . . NO
PRINT OUTPUT CONTROLS . . . . . . . . . . . . .NO PRINTOUT
DATABASE OUTPUT CONTROLS
ITEM FREQUENCY COMPONENT
ALL NONE
NSOL ALL
RSOL ALL
EANG ALL
ETMP ALL
VENG ALL
STRS ALL
EPEL ALL
EPPL ALL
CONT ALL
SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr
*********** PRECISE MASS SUMMARY ***********
TOTAL RIGID BODY MASS MATRIX ABOUT ORIGIN
Translational mass | Coupled translational/rotational mass
138.26 0.0000 0.0000 | 0.0000 -56.527 30.290
0.0000 138.26 0.0000 | 56.527 0.0000 0.75668E-02
0.0000 0.0000 138.26 | -30.290 -0.75668E-02 0.0000
------------------------------------------ | ------------------------------------------
| Rotational mass (inertia)
| 31.206 0.16551E-02 0.31942E-02
| 0.16551E-02 27.750 -12.384
| 0.31942E-02 -12.384 11.101
TOTAL MASS = 138.26
The mass principal axes coincide with the global Cartesian axes
CENTER OF MASS (X,Y,Z)= 0.54728E-04 -0.21908 -0.40884
TOTAL INERTIA ABOUT CENTER OF MASS
1.4602 -0.26388E-05 0.10066E-03
-0.26388E-05 4.6400 0.62632E-06
0.10066E-03 0.62632E-06 4.4655
The inertia principal axes coincide with the global Cartesian axes
*** MASS SUMMARY BY ELEMENT TYPE ***
TYPE MASS
1 100.154
2 19.0543
3 19.0544
Range of element maximum matrix coefficients in global coordinates
Maximum = 1.367915649E+10 at element 35624.
Minimum = 285637981 at element 9309.
*** ELEMENT MATRIX FORMULATION TIMES
TYPE NUMBER ENAME TOTAL ELAPSED AVG ELAPSED
1 34745 SOLID187 1.6845 0.000048481
2 6392 SOLID187 0.3135 0.000049048
3 6561 SOLID187 0.3109 0.000047388
4 396 CONTA174 0.0704 0.000177834
5 370 TARGE170 0.0007 0.000001759
6 380 CONTA174 0.0670 0.000176233
7 371 TARGE170 0.0007 0.000001765
8 1664 SURF154 0.0536 0.000032201
Elapsed Time at end of element matrix formulation = 3.31186056.
DISTRIBUTED SPARSE MATRIX DIRECT SOLVER.
Number of equations = 221211, Maximum wavefront = 552
Memory allocated on only this MPI rank (rank 0)
-------------------------------------------------------------------
Equation solver memory allocated = 441.067 MB
Equation solver memory required for in-core mode = 422.285 MB
Equation solver memory required for out-of-core mode = 126.772 MB
Total (solver and non-solver) memory allocated = 1440.551 MB
Total memory summed across all MPI ranks on this machines
-------------------------------------------------------------------
Equation solver memory allocated = 1623.512 MB
Equation solver memory required for in-core mode = 1554.324 MB
Equation solver memory required for out-of-core mode = 478.227 MB
Total (solver and non-solver) memory allocated = 4005.094 MB
*** NOTE *** ELAPSED TIME = 3.922 TIME= 22:15:46
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= 53280 totEqn= 54953 Job CP sec= 9.692
Factor Done= 51% Factor Wall sec= 0.818 rate= 29.3 GFlops
curEqn= 54953 totEqn= 54953 Job CP sec= 10.427
Factor Done= 100% Factor Wall sec= 1.550 rate= 30.2 GFlops
Distributed sparse solver maximum pivot= 1.734901639E+10 at node 60529
UX.
Distributed sparse solver minimum pivot= 129870096 at node 53832 UY.
Distributed sparse solver minimum pivot in absolute value= 129870096 at
node 53832 UY.
*** ELEMENT RESULT CALCULATION TIMES
TYPE NUMBER ENAME TOTAL ELAPSED AVG ELAPSED
1 34745 SOLID187 1.4349 0.000041297
2 6392 SOLID187 0.2621 0.000041009
3 6561 SOLID187 0.2655 0.000040464
4 396 CONTA174 0.0056 0.000014183
6 380 CONTA174 0.0055 0.000014396
8 1664 SURF154 0.0405 0.000024342
*** NODAL LOAD CALCULATION TIMES
TYPE NUMBER ENAME TOTAL ELAPSED AVG ELAPSED
1 34745 SOLID187 0.3792 0.000010914
2 6392 SOLID187 0.0695 0.000010869
3 6561 SOLID187 0.0702 0.000010693
4 396 CONTA174 0.0003 0.000000882
6 380 CONTA174 0.0003 0.000000908
8 1664 SURF154 0.0027 0.000001612
*** LOAD STEP 1 SUBSTEP 1 COMPLETED. CUM ITER = 1
*** TIME = 1.00000 TIME INC = 1.00000 NEW TRIANG MATRIX
*** MAPDL BINARY FILE STATISTICS
BUFFER SIZE USED= 16384
3.688 MB WRITTEN ON ELEMENT SAVED DATA FILE: file0.esav
35.812 MB WRITTEN ON ASSEMBLED MATRIX FILE: file0.full
8.500 MB WRITTEN ON RESULTS FILE: file0.rst
*************** Write FE CONNECTORS *********
WRITE OUT CONSTRAINT EQUATIONS TO FILE= file.ce
****************************************************
*************** FINISHED SOLVE FOR LS 1 *************
FINISH SOLUTION PROCESSING
***** ROUTINE COMPLETED ***** ELAPSED TIME = 6.874
*GET _WALLASOL FROM ACTI ITEM=TIME WALL VALUE= 0.190960835E-02
PRINTOUT RESUMED BY /GOP
*** MAPDL - ENGINEERING ANALYSIS SYSTEM RELEASE 2026 R1 26.1 ***
Ansys Mechanical Enterprise
00000000 VERSION=LINUX x64 22:15:49 JAN 27, 2026 Elapsed Time= 6.880
--Static Structural
***** MAPDL RESULTS INTERPRETATION (POST1) *****
*** NOTE *** ELAPSED TIME = 6.880 TIME= 22:15:49
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 ***** ELAPSED TIME = 6.880
PRINTOUT RESUMED BY /GOP
*GET _WALLDONE FROM ACTI ITEM=TIME WALL VALUE= 0.191127176E-02
PARAMETER _PREPTIME = 0.2613213347
PARAMETER _SOLVTIME = 6.009784701
PARAMETER _POSTTIME = 0.5988257236E-02
PARAMETER _TOTALTIM = 6.277094293
*GET _DLBRATIO FROM ACTI ITEM=SOLU DLBR VALUE= 1.01186967
*GET _COMBTIME FROM ACTI ITEM=SOLU COMB VALUE= 0.103186360
*GET _SSMODE FROM ACTI ITEM=SOLU SSMM VALUE= 2.00000000
*GET _NDOFS FROM ACTI ITEM=SOLU NDOF VALUE= 221211.000
*GET _SOL_END_TIME FROM ACTI ITEM=SET TIME VALUE= 1.00000000
*IF _sol_end_time ( = 1.00000 ) EQ
1.000000 ( = 1.00000 ) THEN
/FCLEAN COMMAND REMOVING ALL LOCAL FILES
*ENDIF
--- Total number of nodes = 75886
--- Total number of elements = 50879
--- Element load balance ratio = 1.01186967
--- Time to combine distributed files = 0.10318636
--- Sparse memory mode = 2
--- Number of DOF = 221211
EXIT MAPDL WITHOUT SAVING DATABASE
NUMBER OF WARNING MESSAGES ENCOUNTERED= 2
NUMBER OF ERROR MESSAGES ENCOUNTERED= 0
+--------------------- M A P D L S T A T I S T I C S ------------------------+
Release: 2026 R1 Build: 26.1 Update: UP20260112 Platform: LINUX x64
Date Run: 01/27/2026 Time: 22:15 Process ID: 26411
Operating System: Ubuntu 22.04.5 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 5.1.1 Build 20251007
Intel(R) oneAPI Math Kernel Library Version 2024.2-Product Build 20240605
Number of machines requested : 1
Total number of cores available : 16
Number of physical cores available : 8
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 v4.1.8
GPU Acceleration: Not Requested
Job Name: file0
Input File: dummy.dat
Core Machine Name Working Directory
-----------------------------------------------------
0 d42525df87ef /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural
1 d42525df87ef /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural
2 d42525df87ef /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural
3 d42525df87ef /github/home/.mw/Application Data/Ansys/v261/AnsysMech797D/Project_Mech_Files/StaticStructural
Latency time from master to core 1 = 1.850 microseconds
Latency time from master to core 2 = 1.826 microseconds
Latency time from master to core 3 = 1.846 microseconds
Communication speed from master to core 1 = 14042.44 MB/sec
Communication speed from master to core 2 = 16991.00 MB/sec
Communication speed from master to core 3 = 16751.67 MB/sec
Total CPU time for main thread : 6.5 seconds
Total CPU time summed for all threads : 12.8 seconds
Elapsed time spent obtaining a license : 0.4 seconds
Elapsed time spent pre-processing model (/PREP7) : 0.3 seconds
Elapsed time spent solution - preprocessing : 1.4 seconds
Elapsed time spent computing solution : 4.2 seconds
Elapsed time in element formation & assembly : 0.8 seconds
Elapsed time in equation solver : 2.5 seconds
Elapsed time in element result calculations : 0.8 seconds
Elapsed time spent solution - postprocessing : 0.1 seconds
Elapsed time spent post-processing model (/POST1) : 0.0 seconds
Equation solver used : Sparse (symmetric)
Sparse direct equation solver computational rate : 109.1 Gflops
Sparse direct equation solver effective I/O rate : 30.4 GB/sec
Sum of disk space used on all processes : 223.1 MB
Sum of memory used on all processes : 2011.0 MB
Sum of memory allocated on all processes : 4227.0 MB
Physical memory available : 63 GB
Total amount of I/O written to disk : 0.1 GB
Total amount of I/O read from disk : 0.0 GB
+------------------ E N D M A P D L S T A T I S T I C S -------------------+
*-----------------------------------------------------------------------------*
| |
| RUN COMPLETED |
| |
|-----------------------------------------------------------------------------|
| |
| Ansys MAPDL 2026 R1 Build 26.1 UP20260112 LINUX x64 |
| |
|-----------------------------------------------------------------------------|
| |
| Database Requested(-db) 1024 MB Scratch Memory Requested 1024 MB |
| Max Database Used(Master) 62 MB Max Scratch Used(Master) 544 MB |
| Max Database Used(Workers) 1 MB Max Scratch Used(Workers) 484 MB |
| Sum Database Used(All) 65 MB Sum Scratch Used(All) 1946 MB |
| |
|-----------------------------------------------------------------------------|
| |
| CP Time (sec) = 12.825 Time = 22:15:49 |
| Elapsed Time (sec) = 7.102 Date = 01/27/2026 |
| |
*-----------------------------------------------------------------------------*
Print the project tree#
app.print_tree()
├── Project
| ├── Model
| | ├── Geometry Imports (✓)
| | | ├── Geometry Import (✓)
| | ├── Geometry (✓)
| | | ├── Connector
| | | | ├── Connector\Solid1
| | | ├── Right_elbow
| | | | ├── Right_elbow\Solid1
| | | ├── Left_elbow
| | | | ├── Left_elbow\Solid1
| | ├── Materials (✓)
| | | ├── Structural Steel (✓)
| | | ├── Structural Steel Assignment (✓)
| | ├── Coordinate Systems (✓)
| | | ├── Global Coordinate System (✓)
| | ├── Remote Points (✓)
| | ├── Connections (✓)
| | | ├── Contacts (✓)
| | | | ├── Contact Region (✓)
| | | | ├── Contact Region 2 (✓)
| | ├── Mesh (✓)
| | ├── Named Selections
| | | ├── NSFixedSupportFaces (✓)
| | | ├── NSFrictionlessSupportFaces (✓)
| | | ├── NSInsideFaces (✓)
| | ├── Static Structural (✓)
| | | ├── Analysis Settings (✓)
| | | ├── Fixed Support (✓)
| | | ├── Frictionless Support (✓)
| | | ├── Pressure (✓)
| | | ├── Solution (✓)
| | | | ├── Solution Information (✓)
| | | | ├── Total Deformation (✓)
| | | | ├── Equivalent Stress (✓)
Clean up the project#
# Save the project
mechdat_file = output_path / "valve.mechdat"
app.save_as(str(mechdat_file), overwrite=True)
# Close the app
app.close()
# Delete the example files
delete_downloads()
True
Total running time of the script: (0 minutes 25.891 seconds)