# MAPDL 2D Beam ExampleΒΆ

This is an example from FINITE ELEMENT ANALYSIS USING ANSYS 11.0

Launch MAPDL with interactive plotting

```from ansys.mapdl.core import launch_mapdl

mapdl = launch_mapdl()
```

Define an I-beam

```mapdl.prep7()
mapdl.et(1, "BEAM188")
mapdl.keyopt(1, 4, 1)  # transverse shear stress output

# material properties
mapdl.mp("EX", 1, 2e7)  # N/cm2
mapdl.mp("PRXY", 1, 0.27)  #  Poisson's ratio

# beam properties in centimeters
sec_num = 1
mapdl.sectype(sec_num, "BEAM", "I", "ISection", 3)
mapdl.secoffset("CENT")
beam_info = mapdl.secdata(15, 15, 29, 2, 2, 1)  # dimensions are in centimeters
```

Create nodes within MAPDL

```mapdl.n(1, 0, 0, 0)
mapdl.n(12, 110, 0, 0)
mapdl.n(23, 220, 0, 0)
mapdl.fill(1, 12, 10)
mapdl.fill(12, 23, 10)

# list the node coordinates
print(mapdl.mesh.nodes)

# list the node numbers
print(mapdl.mesh.nnum)

# plot the nodes using VTK
mapdl.nplot(vtk=True, nnum=True, cpos="xy", show_bounds=True, point_size=10)
```

Out:

```[[  0.   0.   0.]
[ 10.   0.   0.]
[ 20.   0.   0.]
[ 30.   0.   0.]
[ 40.   0.   0.]
[ 50.   0.   0.]
[ 60.   0.   0.]
[ 70.   0.   0.]
[ 80.   0.   0.]
[ 90.   0.   0.]
[100.   0.   0.]
[110.   0.   0.]
[120.   0.   0.]
[130.   0.   0.]
[140.   0.   0.]
[150.   0.   0.]
[160.   0.   0.]
[170.   0.   0.]
[180.   0.   0.]
[190.   0.   0.]
[200.   0.   0.]
[210.   0.   0.]
[220.   0.   0.]]
[ 1  2  3  4  5  6  7  8  9 10 11 12 13 14 15 16 17 18 19 20 21 22 23]

[(110.0, 0.0, 425.0073635671901),
(110.0, 0.0, 0.0),
(0.0, 1.0, 0.0)]
```

create elements between the nodes we can just manually create elements since we know that the elements are sequential

```for node in mapdl.mesh.nnum[:-1]:
mapdl.e(node, node + 1)

# print the elements from MAPDL
print(mapdl.elist())
```

Out:

```LIST ALL SELECTED ELEMENTS.  (LIST NODES)

*** ANSYS - ENGINEERING ANALYSIS SYSTEM  RELEASE 2021 R2          21.2BETA ***
Ansys Mechanical Enterprise
00000000  VERSION=LINUX x64     15:28:50  JAN 21, 2022 CP=     71.929

** WARNING: PRE-RELEASE VERSION OF ANSYS 21.2BETA
ANSYS,INC TESTING IS NOT COMPLETE - CHECK RESULTS CAREFULLY **

ELEM MAT TYP REL ESY SEC        NODES

1   1   1   1   0   1      1     2     0
2   1   1   1   0   1      2     3     0
3   1   1   1   0   1      3     4     0
4   1   1   1   0   1      4     5     0
5   1   1   1   0   1      5     6     0
6   1   1   1   0   1      6     7     0
7   1   1   1   0   1      7     8     0
8   1   1   1   0   1      8     9     0
9   1   1   1   0   1      9    10     0
10   1   1   1   0   1     10    11     0
11   1   1   1   0   1     11    12     0
12   1   1   1   0   1     12    13     0
13   1   1   1   0   1     13    14     0
14   1   1   1   0   1     14    15     0
15   1   1   1   0   1     15    16     0
16   1   1   1   0   1     16    17     0
17   1   1   1   0   1     17    18     0
18   1   1   1   0   1     18    19     0
19   1   1   1   0   1     19    20     0
20   1   1   1   0   1     20    21     0
21   1   1   1   0   1     21    22     0
22   1   1   1   0   1     22    23     0
```

Access them as a list of arrays See the documentation on `mapdl.mesh.elem` for interperting the individual elements

```for elem in mapdl.mesh.elem:
print(elem)
```

Out:

```[1 1 1 1 0 0 0 0 0 0 1 2 0]
[1 1 1 1 0 0 0 0 0 0 2 3 0]
[1 1 1 1 0 0 0 0 0 0 3 4 0]
[1 1 1 1 0 0 0 0 0 0 4 5 0]
[1 1 1 1 0 0 0 0 0 0 5 6 0]
[1 1 1 1 0 0 0 0 0 0 6 7 0]
[1 1 1 1 0 0 0 0 0 0 7 8 0]
[1 1 1 1 0 0 0 0 0 0 8 9 0]
[ 1  1  1  1  0  0  0  0  0  0  9 10  0]
[ 1  1  1  1  0  0  0  0  0  0 10 11  0]
[ 1  1  1  1  0  0  0  0  0  0 11 12  0]
[ 1  1  1  1  0  0  0  0  0  0 12 13  0]
[ 1  1  1  1  0  0  0  0  0  0 13 14  0]
[ 1  1  1  1  0  0  0  0  0  0 14 15  0]
[ 1  1  1  1  0  0  0  0  0  0 15 16  0]
[ 1  1  1  1  0  0  0  0  0  0 16 17  0]
[ 1  1  1  1  0  0  0  0  0  0 17 18  0]
[ 1  1  1  1  0  0  0  0  0  0 18 19  0]
[ 1  1  1  1  0  0  0  0  0  0 19 20  0]
[ 1  1  1  1  0  0  0  0  0  0 20 21  0]
[ 1  1  1  1  0  0  0  0  0  0 21 22  0]
[ 1  1  1  1  0  0  0  0  0  0 22 23  0]
```

Define the boundary conditions

```# Allow movement only in the X and Z direction
for const in ["UX", "UY", "ROTX", "ROTZ"]:
mapdl.d("all", const)

# constrain just nodes 1 and 23 in the Z direction
mapdl.d(1, "UZ")
mapdl.d(23, "UZ")

# apply a -Z force at node 12
mapdl.f(12, "FZ", -22840)
```

Out:

```'SPECIFIED NODAL LOAD FZ   FOR SELECTED NODES        12 TO       12 BY        1\n  REAL= -22840.0000       IMAG=  0.00000000'
```

run the static analysis

```mapdl.run("/solu")
mapdl.antype("static")
print(mapdl.solve())
```

Out:

```*****  ANSYS SOLVE    COMMAND  *****

*** NOTE ***                            CP =      71.934   TIME= 15:28:50
There is no title defined for this analysis.

*** SELECTION OF ELEMENT TECHNOLOGIES FOR APPLICABLE ELEMENTS ***
---GIVE SUGGESTIONS ONLY---

ELEMENT TYPE         1 IS BEAM188 . KEYOPT(1)=1 IS SUGGESTED FOR NON-CIRCULAR CROSS
SECTIONS AND KEYOPT(3)=2 IS ALWAYS SUGGESTED.

ELEMENT TYPE         1 IS BEAM188 . KEYOPT(15) IS ALREADY SET AS SUGGESTED.

*** ANSYS - ENGINEERING ANALYSIS SYSTEM  RELEASE 2021 R2          21.2BETA ***
Ansys Mechanical Enterprise
00000000  VERSION=LINUX x64     15:28:50  JAN 21, 2022 CP=     71.935

** WARNING: PRE-RELEASE VERSION OF ANSYS 21.2BETA
ANSYS,INC TESTING IS NOT COMPLETE - CHECK RESULTS CAREFULLY **

S O L U T I O N   O P T I O N S

PROBLEM DIMENSIONALITY. . . . . . . . . . . . .3-D
DEGREES OF FREEDOM. . . . . . UX   UY   UZ   ROTX ROTY ROTZ
ANALYSIS TYPE . . . . . . . . . . . . . . . . .STATIC (STEADY-STATE)
GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC

*** NOTE ***                            CP =      71.935   TIME= 15:28:50
Present time 0 is less than or equal to the previous time.  Time will
default to 1.

*** NOTE ***                            CP =      71.935   TIME= 15:28:50
The conditions for direct assembly have been met.  No .emat or .erot
files will be produced.

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. . . . . . . . . . . .ALL DATA WRITTEN
FOR THE LAST SUBSTEP

SOLUTION MONITORING INFO IS WRITTEN TO FILE= file.mntr

*** NOTE ***                            CP =      71.940   TIME= 15:28:50
Predictor is ON by default for structural elements with rotational
degrees of freedom.  Use the PRED,OFF command to turn the predictor
OFF if it adversely affects the convergence.

Range of element maximum matrix coefficients in global coordinates
Maximum = 2.504767151E+10 at element 22.
Minimum = 2.504767151E+10 at element 22.

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

1        22  BEAM188       0.009   0.000396
Time at end of element matrix formulation CP = 71.945488.

SPARSE MATRIX DIRECT SOLVER.
Number of equations =          44,    Maximum wavefront =     12
Memory allocated for solver              =     0.065 MB
Memory required for in-core solution     =     0.062 MB
Memory required for out-of-core solution =     0.062 MB

*** NOTE ***                            CP =      71.949   TIME= 15:28:50
The 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.
Sparse solver maximum pivot= 5.009534302E+10 at node 8 ROTY.
Sparse solver minimum pivot= 2691965.06 at node 12 UZ.
Sparse solver minimum pivot in absolute value= 2691965.06 at node 12
UZ.

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

1        22  BEAM188       0.027   0.001225

TYPE    NUMBER   ENAME      TOTAL CP  AVE CP

1        22  BEAM188       0.001   0.000050
*** LOAD STEP     1   SUBSTEP     1  COMPLETED.    CUM ITER =      1
*** TIME =   1.00000         TIME INC =   1.00000      NEW TRIANG MATRIX

*** ANSYS BINARY FILE STATISTICS
BUFFER SIZE USED= 16384
0.062 MB WRITTEN ON ASSEMBLED MATRIX FILE: file.full
0.625 MB WRITTEN ON RESULTS FILE: file.rst
```

Total running time of the script: ( 0 minutes 0.495 seconds)

Gallery generated by Sphinx-Gallery