# Thermal-structural analysis of exhaust manifold#

Summary: This example illustrates how to map results from a CFD analysis and perform a Finite Element (FE) analysis.

## Objective#

In this example, we will perform an FE analysis to compute the thermal stresses developed in an exhaust manifold. The manifold is made of structural steel and the temperature distribution in it is obtained from a CFD run. We import this data and map it onto FE mesh to define thermal load at each node using Gaussian interpolation kernel.

## Procedure#

• Launch MAPDL instance

• Import geometry, assign material properties, and generate FE mesh.

• Import temperature distribution and map it on FE mesh

• Define BCs and use imported temperature distribution to define thermal load.

• Solve the model and plot the results of interest.

## Additional Packages used#

• Numpy for using data as arrays

• Pandas to import csv file (to install use: pip install pandas)

• PyVista for performing Gaussian interpolation

## Boundary Conditions#

• Highlighted faces are fully constrained.

## Import all necessary modules and launch an instance of MAPDL#

```import numpy as np
import pandas as pd
import pyvista as pv

from ansys.mapdl.core import launch_mapdl

# start mapdl
mapdl = launch_mapdl()
print(mapdl)
```
```Product:             Ansys Mechanical Enterprise
MAPDL Version:       22.2
ansys.mapdl Version: 0.64.0
```

## Import geometry, assign material properties and generate a mesh.#

```# download the necessary files
geometry = paths["geometry"]
mapping_data = paths["mapping_data"]

# reset mapdl & import geometry
mapdl.clear()
mapdl.input(geometry)

# Define element attributes
# Second-order tetrahedral elements (SOLID187)
mapdl.prep7()
mapdl.et(1, "SOLID187")

# Define material properties of structural steel
E = 2e11  # Youngs modulus
NU = 0.3  # Poisson's ratio
CTE = 1.2e-5  # Coeff. of thermal expansion
mapdl.mp("EX", 1, E)
mapdl.mp("PRXY", 1, NU)
mapdl.mp("ALPX", 1, CTE)

# Define mesh controls and generate mesh
mapdl.esize(0.0075)
mapdl.vmesh("all")

# Save mesh as VTK object
print(mapdl.mesh)
grid = mapdl.mesh.grid  # save mesh as a VTK object
```
```ANSYS Mesh
Number of Nodes:              87577
Number of Elements:           44241
Number of Element Types:      1
Number of Node Components:    0
Number of Element Components: 0
```

## Import and map temperature data to FE mesh#

```# Import csv file and save data to a NumPy array
temperature_data = temperature_file.values  # Save data to a NumPy array
nd_temp_data = temperature_data[1:, 1:].astype(float)  # Change data type to Float

# Map temperature data to FE mesh
# Convert imported data into PolyData format
wrapped = pv.PolyData(nd_temp_data[:, :3])  # Convert NumPy array to PolyData format
wrapped["temperature"] = nd_temp_data[
:, 3
]  # Add a scalar variable 'temperature' to PolyData

# Perform data mapping
inter_grid = grid.interpolate(
wrapped,
sharpness=5,
strategy="closest_point",
progress_bar=True,
)  # Map the imported data to MAPDL grid
inter_grid.plot(show_edges=False)  # Plot the interpolated data on MAPDL grid
pv.convert_array(inter_grid.active_scalars)
)  # Save temperatures interpolated to each node as NumPy array
node_num = inter_grid.point_data["ansys_node_num"]  # Save node numbers as NumPy array
```
```  0%|          [00:00<?]
Interpolating:   0%|          [00:00<?]
Interpolating: 100%|##########[00:00<00:00]
Interpolating: 100%|##########[00:00<00:00]
Interpolating: 100%|##########[00:00<00:00]
```

## Apply loads and boundary conditions and solve the model#

```# Read all nodal coords. to an array & extract the X and Y min. bounds
array_nodes = mapdl.mesh.nodes
Xmin = np.amin(array_nodes[:, 0])
Ymin = np.amin(array_nodes[:, 1])

# Enter /SOLU processor to apply loads and BCs
mapdl.finish()
mapdl.slashsolu()

# Enter non-interactive mode to assign thermal load at each node using imported data
with mapdl.non_interactive:
for node, temp in zip(node_num, temperature_load_val):
mapdl.bf(node, "TEMP", temp)
# Use the X and Y min. bounds to select nodes from five surfaces that are to be fixed and created a component and fix all DOFs.
mapdl.nsel("s", "LOC", "X", Xmin)  # Select all nodes whose X coord.=Xmin
mapdl.nsel(
"a", "LOC", "Y", Ymin
)  # Select all nodes whose Y coord.=Ymin and add to previous selection
mapdl.cm("fixed_nodes", "NODE")  # Create a nodal component 'fixed_nodes'
mapdl.allsel()  # Revert active selection to full model
mapdl.d(
"fixed_nodes", "all", 0
)  # Impose fully fixed constraint on component created earlier

# Solve the model
output = mapdl.solve()
print(output)
```
```*****  MAPDL SOLVE    COMMAND  *****

*** WARNING ***                         CP =       0.000   TIME= 00:00:00
Previous testing revealed that 127 of the 44241 selected elements
violate shape warning limits.  To review warning messages, please see
the output or error file, or issue the CHECK command.

*** NOTE ***                            CP =       0.000   TIME= 00:00:00
The model data was checked and warning messages were found.
Please review output or errors file ( ) for these warning messages.

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

ELEMENT TYPE         1 IS SOLID187. IT IS NOT ASSOCIATED WITH FULLY INCOMPRESSIBLE
HYPERELASTIC MATERIALS. NO SUGGESTION IS AVAILABLE.

*****MAPDL VERIFICATION RUN ONLY*****
DO NOT USE RESULTS FOR PRODUCTION

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)
GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC

*** NOTE ***                            CP =       0.000   TIME= 00:00:00
Present time 0 is less than or equal to the previous time.  Time will
default to 1.

*** NOTE ***                            CP =       0.000   TIME= 00:00:00
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

Range of element maximum matrix coefficients in global coordinates
Maximum = 1.875024228E+11 at element 0.
Minimum = 313199579 at element 0.

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

1     44241  SOLID187      0.000   0.000000
Time at end of element matrix formulation CP = 0.

SPARSE MATRIX DIRECT SOLVER.
Number of equations =      251853,    Maximum wavefront =      0
Memory available (MB) =    0.0    ,  Memory required (MB) =    0.0

Sparse solver maximum pivot= 0 at node 0 .
Sparse solver minimum pivot= 0 at node 0 .
Sparse solver minimum pivot in absolute value= 0 at node 0 .

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

1     44241  SOLID187      0.000   0.000000

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

1     44241  SOLID187      0.000   0.000000
*** LOAD STEP     1   SUBSTEP     1  COMPLETED.    CUM ITER =      1
*** TIME =   1.00000         TIME INC =   1.00000      NEW TRIANG MATRIX
```

## Post-processing#

```# Enter post-processor
mapdl.post1()
mapdl.set(1, 1)  # Select first load step
mapdl.post_processing.plot_nodal_eqv_stress()  # Plot equivalent stress
```

## Exit MAPDL instance#

```mapdl.exit()
```

Total running time of the script: ( 0 minutes 34.344 seconds)

Gallery generated by Sphinx-Gallery