Note
Go to the end to download the full example code
使用 PyMAPDL 的 DPF-Core 基本用法#
本例改编自 DPF-Core 基本用法示例 ， 展示了如何在 DPF 中打开结果文件，并进行一些基本的后处理。
如果安装了 Ansys 2021 R1，启动 DPF 就非常简单了，因为 DPF-Core 会负责启动后处理 Ansys 文件所需的所有服务。
首先，以 dpf_core 的形式导入 DPF-Core 模块，并导入随附的示例文件。
import tempfile
from ansys.dpf import core as dpf
from ansys.mapdl.core import launch_mapdl
from ansys.mapdl.core.examples import vmfiles
Create model#
运行 MAPDL 验证手册中的示例
mapdl = launch_mapdl()
vm5 = vmfiles["vm5"]
output = mapdl.input(vm5)
print(output)
# 如果在本地工作，则无需执行以下步骤
temp_directory = tempfile.gettempdir()
print(f'默认临时文件地址： {temp_directory}')
# 将 RST 文件下载到当前文件夹
rst_path = mapdl.download_result(temp_directory)
C:\Users\ff\AppData\Local\Programs\Python\Python310\lib\site-packages\ansys\tools\path\path.py:818: DeprecationWarning: This method is going to be deprecated in future versions. Please use 'get_mapdl_path'.
warnings.warn(
/INPUT FILE= C:\Users\ff\AppData\Local\Programs\Python\Python310\lib\site-packages\ansys\mapdl\core\examples\verif\vm5.dat LINE= 0
ANSYS MEDIA REL. 2023R1 (11/04/2022) REF. VERIF. MANUAL: REL. 2023R1
*** VERIFICATION RUN - CASE VM5 *** OPTION= 4
/SHOW SWITCH PLOTS TO JPEG - RASTER MODE.
*****MAPDL VERIFICATION RUN ONLY*****
DO NOT USE RESULTS FOR PRODUCTION
***** MAPDL ANALYSIS DEFINITION (PREP7) *****
TITLE=
VM5, LATERALLY LOADED TAPERED SUPPORT STRUCTURE (QUAD. ELEMENTS)
C*** MECHANICS OF SOLIDS, CRANDALL AND DAHL, 1959, PAGE 342, PROB. 7.18
C*** USING PLANE42 ELEMENTS
PERFORM A STATIC ANALYSIS
THIS WILL BE A NEW ANALYSIS
ELEMENT TYPE 1 IS PLANE182 2-D 4-NODE PLANE STRS SOLID
KEYOPT( 1- 6)= 2 0 3 0 0 0
KEYOPT( 7-12)= 0 0 0 0 0 0
KEYOPT(13-18)= 0 0 0 0 0 0
CURRENT NODAL DOF SET IS UX UY
TWO-DIMENSIONAL MODEL
REAL CONSTANT SET 1 ITEMS 1 TO 6
2.0000 0.0000 0.0000 0.0000 0.0000 0.0000
MATERIAL 1 EX = 0.3000000E+08
MATERIAL 1 NUXY = 0.000000
NODE 1 KCS= 0 X,Y,Z= 25.000 0.0000 0.0000
NODE 7 KCS= 0 X,Y,Z= 75.000 0.0000 0.0000
FILL 5 POINTS BETWEEN NODE 1 AND NODE 7
START WITH NODE 2 AND INCREMENT BY 1
NODE 8 KCS= 0 X,Y,Z= 25.000 -3.0000 0.0000
NODE 14 KCS= 0 X,Y,Z= 75.000 -9.0000 0.0000
FILL 5 POINTS BETWEEN NODE 8 AND NODE 14
START WITH NODE 9 AND INCREMENT BY 1
ELEMENT 1 2 1 8 9
GENERATE 6 TOTAL SETS OF ELEMENTS WITH NODE INCREMENT OF 1
SET IS SELECTED ELEMENTS IN RANGE 1 TO 1 IN STEPS OF 1
MAXIMUM ELEMENT NUMBER= 6
SELECT FOR ITEM=LOC COMPONENT=X BETWEEN 75.000 AND 75.000
KABS= 0. TOLERANCE= 0.375000
2 NODES (OF 14 DEFINED) SELECTED BY NSEL COMMAND.
SPECIFIED CONSTRAINT UX FOR SELECTED NODES 1 TO 14 BY 1
REAL= 0.00000000 IMAG= 0.00000000
ADDITIONAL DOFS= UY
ALL SELECT FOR ITEM=NODE COMPONENT=
IN RANGE 1 TO 14 STEP 1
14 NODES (OF 14 DEFINED) SELECTED BY NSEL COMMAND.
SPECIFIED NODAL LOAD FY FOR SELECTED NODES 1 TO 1 BY 1
REAL= -4000.00000 IMAG= 0.00000000
***** ROUTINE COMPLETED ***** CP = 0.000
***** MAPDL SOLUTION ROUTINE *****
PRINT BASI ITEMS WITH A FREQUENCY OF 1
FOR ALL APPLICABLE ENTITIES
/OUTPUT FILE=
默认临时文件地址： C:\Users\ff\AppData\Local\Temp
接下来，打开生成的 RST 文件并打印出 Model 对象。
Model 类通过跟踪结果文件使用的运算符和数据源，有助于组织结果的访问方法。
打印模型显示：
Analysis type 分析类型
Available results 可用结果
Size of the mesh 网格尺寸
Number of results 结果数量
如果要使用远程服务器，可能需要先上传 RST 文件，然后再使用它。
然后你就可以创建 DPF Model 。
DPF Model
------------------------------
Static analysis
Unit system: SI: m, kg, s, V, A, K
Physics Type: Mechanical
Available results:
- displacement: Nodal Displacement
- reaction_force: Nodal Force
- element_nodal_forces: ElementalNodal Element nodal Forces
- stress: ElementalNodal Stress
- elemental_volume: Elemental Volume
- stiffness_matrix_energy: Elemental Energy-stiffness matrix
- artificial_hourglass_energy: Elemental Hourglass Energy
- thermal_dissipation_energy: Elemental thermal dissipation energy
- kinetic_energy: Elemental Kinetic Energy
- co_energy: Elemental co-energy
- incremental_energy: Elemental incremental energy
- elastic_strain: ElementalNodal Strain
- thermal_strain: ElementalNodal Thermal Strains
- thermal_strains_eqv: ElementalNodal Thermal Strains eqv
- swelling_strains: ElementalNodal Swelling Strains
- structural_temperature: ElementalNodal Temperature
------------------------------
DPF Meshed Region:
33 nodes
6 elements
Unit:
With shell (2D) elements, shell (3D) elements
------------------------------
DPF Time/Freq Support:
Number of sets: 1
Cumulative Time (s) LoadStep Substep
1 1.000000 1 1
Model Metadata#
可以通过引用模型的 metadata 属性从模型中提取特定元数据。
例如，只打印 result_info 属性：
metadata = model.metadata
print(metadata.result_info)
Static analysis
Unit system: SI: m, kg, s, V, A, K
Physics Type: Mechanical
Available results:
- displacement: Nodal Displacement
- reaction_force: Nodal Force
- element_nodal_forces: ElementalNodal Element nodal Forces
- stress: ElementalNodal Stress
- elemental_volume: Elemental Volume
- stiffness_matrix_energy: Elemental Energy-stiffness matrix
- artificial_hourglass_energy: Elemental Hourglass Energy
- thermal_dissipation_energy: Elemental thermal dissipation energy
- kinetic_energy: Elemental Kinetic Energy
- co_energy: Elemental co-energy
- incremental_energy: Elemental incremental energy
- elastic_strain: ElementalNodal Strain
- thermal_strain: ElementalNodal Thermal Strains
- thermal_strains_eqv: ElementalNodal Thermal Strains eqv
- swelling_strains: ElementalNodal Swelling Strains
- structural_temperature: ElementalNodal Temperature
打印 mesh region（网格区域） ：
print(metadata.meshed_region)
DPF Meshed Region:
33 nodes
6 elements
Unit:
With shell (2D) elements, shell (3D) elements
要打印结果的时间或频率，请使用 time_freq_support：
print(metadata.time_freq_support)
DPF Time/Freq Support:
Number of sets: 1
Cumulative Time (s) LoadStep Substep
1 1.000000 1 1
Extracting Displacement Results#
可以通过 Results 属性访问模型的所有结果，
该属性返回 ansys.dpf.core.results.Results 类。该类包含特定结果文件可用的 DPF 结果运算符，使用 print(results) 打印对象时会列出这些运算符。
这里，displacement 运算符与 DataSources（数据源） 相联，
这会在运行 results.displacement() 时自动进行。
默认情况下，displacement 运算符连接到第一个结果集，对于此静态结果而言，它是唯一的结果。
results = model.results
displacements = results.displacement()
fields = displacements.outputs.fields_container()
# 最后，提取位移场数据：
disp = fields[0].data
disp
DPFArray([[-4.38851905e-03, -8.90023185e-03, 0.00000000e+00],
[-6.69683824e-03, -2.11175625e-02, 0.00000000e+00],
[ 4.17859820e-03, -2.11057663e-02, 0.00000000e+00],
[ 3.30502628e-03, -8.89049154e-03, 0.00000000e+00],
[-5.53644478e-03, -1.42612890e-02, 0.00000000e+00],
[-1.20792265e-03, -2.11145211e-02, 0.00000000e+00],
[ 3.82436228e-03, -1.42559816e-02, 0.00000000e+00],
[-4.90502176e-04, -8.89780417e-03, 0.00000000e+00],
[-2.17801557e-03, -2.15151386e-03, 0.00000000e+00],
[ 1.82830253e-03, -2.15124124e-03, 0.00000000e+00],
[-3.27160527e-03, -4.90756375e-03, 0.00000000e+00],
[ 2.63019818e-03, -4.89004246e-03, 0.00000000e+00],
[-8.95838911e-05, -2.15503538e-03, 0.00000000e+00],
[ 0.00000000e+00, 0.00000000e+00, 0.00000000e+00],
[ 0.00000000e+00, 0.00000000e+00, 0.00000000e+00],
[-1.07316284e-03, -5.41584305e-04, 0.00000000e+00],
[ 9.59021573e-04, -5.64429271e-04, 0.00000000e+00],
[ 0.00000000e+00, 0.00000000e+00, 0.00000000e+00],
[-1.10106159e-02, -6.60224200e-02, 0.00000000e+00],
[-1.20838957e-02, -9.90994350e-02, 0.00000000e+00],
[ 3.61860276e-04, -9.88721453e-02, 0.00000000e+00],
[ 3.23207196e-03, -6.59380057e-02, 0.00000000e+00],
[-1.17563515e-02, -8.18061655e-02, 0.00000000e+00],
[-5.82220244e-03, -9.89754713e-02, 0.00000000e+00],
[ 2.08036965e-03, -8.18682795e-02, 0.00000000e+00],
[-3.87518431e-03, -6.59854725e-02, 0.00000000e+00],
[-8.99066833e-03, -3.98506343e-02, 0.00000000e+00],
[ 4.27062988e-03, -3.98210573e-02, 0.00000000e+00],
[-1.00608366e-02, -5.19510806e-02, 0.00000000e+00],
[ 3.92601832e-03, -5.19563394e-02, 0.00000000e+00],
[-2.31550786e-03, -3.98370089e-02, 0.00000000e+00],
[-7.85485340e-03, -2.95981071e-02, 0.00000000e+00],
[ 4.34038437e-03, -2.95942670e-02, 0.00000000e+00]])
Plot displacements#
您可以使用以下方法打印上面的位移场：
model.metadata.meshed_region.plot(fields, cpos="xy")
或使用
fields[0].plot(cpos="xy")
如果您在网格或结果上使用了 ansys.dpf.core.scoping.Scoping 方法，这种方法会特别有用。
Close session#
Stop MAPDL session.
mapdl.exit()
Total running time of the script: (0 minutes 9.507 seconds)