Postprocessing TACS Solutions

TACS provides comprehensive postprocessing capabilities through its native f5 file format and conversion utilities. This section explains how to generate f5 files from TACS analyses and convert them to standard visualization formats for detailed analysis and presentation.

Overview

The TACS postprocessing workflow consists of three main steps:

1. Generate f5 files from your TACS analysis containing solution data

2. Convert f5 files to standard visualization formats (Tecplot or ParaView)

3. Visualize and analyze results using your preferred visualization software

F5 File Format

TACS uses the f5 file format (based on HDF5) to store solution data in a parallel, binary format. F5 files contain both continuous (nodal) and element-wise data, making them suitable for detailed postprocessing and visualization.

Creating F5 Files

Method 1: Using the Direct (C++) Interface

To create an f5 file from a TACS analysis, use the TACSToFH5 class. This should be done after solving your analysis but before cleaning up the assembler object.

#include "TACSToFH5.h"

// After solving your analysis
// Create an TACSToFH5 object for writing output to files
ElementType etype = TACS_BEAM_OR_SHELL_ELEMENT;
int write_flag = (TACS_OUTPUT_CONNECTIVITY | TACS_OUTPUT_NODES |
                  TACS_OUTPUT_DISPLACEMENTS | TACS_OUTPUT_STRAINS |
                  TACS_OUTPUT_STRESSES | TACS_OUTPUT_EXTRAS);
TACSToFH5 *f5 = new TACSToFH5(assembler, etype, write_flag);
f5->incref();
f5->writeToFile("solution.f5");
f5->decref();

Tip

The ElementType should match the type of elements in your model. Common types include:

• TACS_BEAM_OR_SHELL_ELEMENT for shell and beam elements

• TACS_SOLID_ELEMENT for 3D solid elements

• TACS_PLANE_STRESS_ELEMENT for 2D plane stress elements

Method 2: Using the pyTACS (Python) interface

To create an f5 file from a TACS analysis, use the writeSolution method of any problem class after solving the problem.

from tacs import pyTACS, TACS
bdfFile = "input.bdf"
options = {# Specify the element type to output in f5 file
           # If not specified, pyTACS will choose this option automatically
           # based on first element type in model
           "outputElement": TACS.BEAM_OR_SHELL_ELEMENT,
           # Output flags
           "writeConnectivity": True,
           "writeNodes": True,
           "writeDisplacements": True,
           "writeStrains": True,
           "writeStresses": True,
           "writeExtras": True}
FEAAssembler = pyTACS(bdfFile, options=options)
FEAAssembler.initialize()
# Creata a pytacs problem
staticProb = FEAAssembler.createStaticProblem("grav")
staticProb.addInertialLoad([0.0, 0.0, -9.81])
# Solve
staticProb.solve()
# Write the solution to an f5 file
FEAAssembler.writeSolution()

Output Flags

The following output flags control what data is written to the f5 file. The table shows both the C++ interface flags and their equivalent pyTACS options. You can combine multiple C++ flags using the bitwise OR operator (|), while pyTACS options are set as boolean values in the options dictionary when the pyTACS object is created:

Output Flags

Direct (C++) Flag	pyTACS (Python) Option	Description
TACS_OUTPUT_CONNECTIVITY	writeConnectivity	Element connectivity information (required for visualization)
TACS_OUTPUT_NODES	writeNodes	Nodal coordinates (X, Y, Z) - essential for geometry visualization
TACS_OUTPUT_DISPLACEMENTS	writeDisplacements	Nodal displacements and rotations - needed for deformed shape visualization
TACS_OUTPUT_STRAINS	writeStrains	Element strains - useful for strain analysis and contour plots
TACS_OUTPUT_STRESSES	writeStresses	Element stresses - essential for stress analysis and failure assessment
TACS_OUTPUT_EXTRAS	writeExtras	Additional quantities (failure indices, design variables) - useful for optimization
TACS_OUTPUT_LOADS	writeLoads	Applied loads - helpful for load verification and visualization
TACS_OUTPUT_COORDINATE_FRAME	writeCoordinateFrame	Element coordinate frames - useful for composite material analysis

Note

For basic visualization, you typically need at least TACS_OUTPUT_CONNECTIVITY, TACS_OUTPUT_NODES, and TACS_OUTPUT_DISPLACEMENTS. Add other flags based on your analysis requirements.

Converting F5 Files

TACS provides two utilities for converting f5 files to standard visualization formats. These utilities are typically located in the extern/ directory of your TACS installation.

f5totec: Convert to Tecplot Format

The f5totec utility converts f5 files to Tecplot format (.plt files):

# Basic conversion
f5totec solution.f5

This creates a solution.plt file that can be opened in Tecplot.

f5tovtk: Convert to VTK Format

The f5tovtk utility converts f5 files to VTK format (.vtk files) for use with ParaView:

# Basic conversion
f5tovtk solution.f5

This creates a solution.vtk file that can be opened in ParaView.

Note

When a node is used by multiple elements, each element may have a different value for variables such as stress, strain, failure criteria, and design variables at that node. f5totec produces a single value for each node by averaging the values from each element. This can lead to unrealistic values of these variables in certain situations (e.g design variable values at the boundaries between different components and stress/strain/failure criteria values at points where shell elements meet at very different orientations.

Troubleshooting Conversion Issues:

• Ensure the f5 file was generated successfully and contains the expected data

• Check that the conversion utilities are compiled and accessible in your PATH

Output Variables by Element Type

The following tables describe the output variables available for each element type in TACS.

Tip

For elements that have a local coordinate system (e.g shells and beams), the stress and strain outputs are in the local coordinate system. For example, ex0/sx0 are in the direction of the local reference axis, ey0/sy0 are in the direction of the second reference frame vector. Other variables, such as forces fx, fy, fz are given in the global reference frame.

Beam/Shell Elements (TACS_BEAM_OR_SHELL_ELEMENT)

Beam/Shell Element Output Variables

Category	Variable	Description
Displacements	u, v, w	Translational displacements
	rotx, roty, rotz	Rotational displacements
Strains	ex0, ey0, exy0	Membrane strains
	ex1, ey1, exy1	Bending strains
	eyz0, exz0	Transverse shear strains
	erot	Drilling strain
Stresses	sx0, sy0, sxy0	Membrane stress resultants
	sx1, sy1, sxy1	Bending stress resultants
	syz0, sxz0	Transverse shear stress resultants
	srot	Drilling stress resultant
Extras	failure0-failure6	Failure indices for different failure criteria
	dv1-dv7	Design variables
Loads	fx, fy, fz	Applied forces
	mx, my, mz	Applied moments
Coordinate Frame	t0x, t0y, t0z	First element reference frame vector (i.e. reference axis) components
	t1x, t1y, t1z	Second element reference frame vector components
	t2x, t2y, t2z	Third element reference frame vector (i.e. normal vector) components

Solid Elements (TACS_SOLID_ELEMENT)

Solid Element Output Variables

Category	Variable	Description
Displacements	u, v, w	Translational displacements
Strains	exx, eyy, ezz	Normal strains
	gyz, gxz, gxy	Shear strains
Stresses	sxx, syy, szz	Normal stresses
	syz, sxz, sxy	Shear stresses
Extras	failure	Failure index
	dv1, dv2, dv3	Design variables
Loads	fx, fy, fz	Applied forces

Plane Stress Elements (TACS_PLANE_STRESS_ELEMENT)

Plane Stress Element Output Variables

Category	Variable	Description
Displacements	u, v	In-plane displacements
Strains	exx, eyy, gxy	In-plane strains
Stresses	sxx, syy, sxy	In-plane stresses
Extras	failure	Failure index
	dv1, dv2, dv3	Design variables
Loads	fx, fy	Applied forces

Scalar Elements (TACS_SCALAR_2D_ELEMENT, TACS_SCALAR_3D_ELEMENT)

Scalar Element Output Variables

Category	Variable	Description
Displacements	u	Scalar displacement
Strains	ux, uy (2D) / ux, uy, uz (3D)	Gradient components
Stresses	sx, sy (2D) / sx, sy, sz (3D)	Flux components
Extras	failure	Failure index
	dv1, dv2, dv3	Design variables
Loads	f	Applied load

PCM Elements (TACS_PCM_ELEMENT)

PCM Element Output Variables

Category	Variable	Description
Displacements	dT	Temperature change
Strains	gradx, grady	Temperature gradient components
Stresses	fluxx, fluxy	Heat flux components
Extras	rho	Density
	dv1, dv2, dv3	Design variables
	phase	Phase field
Loads	Q	Applied heat source

Visualization Tips

1. Element-wise vs. Nodal Data: F5 files contain both element-wise and nodal data. The conversion utilities automatically perform nodal averaging for element-wise quantities.

2. Higher-order Elements: Higher-order elements are split into multiple lower order element for visualization (e.g., each quadratic triangle becomes 3 linear triangles).

3. Component Separation: In Tecplot, each component in the model can be written as a separate zone in the output files, making it easy to visualize different parts of the structure.

Visualizing Deformed Surfaces

One of the most common postprocessing tasks is visualizing the deformed shape of structures. TACS provides both nodal coordinates (X, Y, Z) and displacements (u, v, w) that can be used to create deformed surface visualizations.

Creating Deformed Geometry in Tecplot

In Tecplot, you can visualize deformed surfaces by creating new variables that represent the deformed coordinates:

1. Open the converted .plt file in Tecplot

2. Create new variables for deformed coordinates:

   • Go to Data > Alter > Specify Equations

   • Under the Equations box enter:

     {XDEF} = {X} + {u}
     {YDEF} = {Y} + {v}
     {ZDEF} = {Z} + {w}
     

3. Create the deformed plot:

   • Go to Plot > Assign XYZ...

   • Set X, Y, Z to XDEF, YDEF, ZDEF

   • Choose appropriate surface rendering (Surface, Mesh, or Contour)

Tecplot Macro

You can also automate this process using a Tecplot macro. Place this code in your tecplot.mcr file to make it available as a quick macro in the Tecplot GUI:

$!MACROFUNCTION NAME = "TACS - Apply Deformations"
$!PromptForTextString |DefFactor|
  Instructions = "Enter scaling factor for deformations"

$!AlterData
  Equation = "{X}={X}+|DefFactor|*{u}"
$!AlterData
  Equation = "{Y}={Y}+|DefFactor|*{v}"
$!AlterData
  Equation = "{Z}={Z}+|DefFactor|*{w}"
$!ENDMACROFUNCTION

Note that this macro modifies the original X, Y, Z variables, rather than creating new variables for the deformed coordinates as is done above.

Creating Deformed Geometry in ParaView

ParaView provides several methods to visualize deformed surfaces:

1. Open the converted .vtk file in ParaView

2. Add Calculator filter: - Select the dataset - Go to Filters > Alphabetical > Calculator

3. Create deformed coordinates:

   • Set Result Array Name to def_vec

   • Set Function to u*iHat + v*jHat + w*kHat

   • Click Apply

4. Add Warp By Vector filter:

   • Select the dataset

   • Go to Filters > Alphabetical > Warp By Vector

5. Configure the warp:

   • Set Vector to def_vec

   • Adjust Scale Factor to control deformation magnification

   • Click Apply