Rob Siegwart - FEA

FEA Basics and Development of a 2D Link Element

2021-06-17T00:00:00-05:00

In my quest to learn more about the inner workings of the finite element method and its programming implementation, I have started off attempting to program the simplest of FEA models and analyses via the direct stiffness method. (Here is my work so far on the topic of this article - simpleFEA.)

To that end, a 2D link or truss element is probably the simplest finite element there is (maybe besides a point mass).

Concepts

Big Picture

The basics of a linear structural FEA is the stiffness equation:

\begin{equation*} \mathbf{F} = \mathbf{K}\mathbf{U} \end{equation*}

where \(\mathbf{F}\) is the global force vector, \(\mathbf{K}\) the global stiffness matrix, and \(\mathbf{U}\) the global displacement vector. The size of this system (length of vector) is equal to the total number of nodal degrees-of-freedom (DOF). The goal of the linear finite element program therefore is to assemble and solve this system of equations.

The matrix form of this equation represents the interrelation of the connectivity of nodes by elements. If expanded, each row would contain only those nodes that contribute to the force term of that row. And, a node typically is only connected to a few elements and because there are usually a large number of elements, this matrix contains many empty/zero entries. (This leads to the concept of sparse matrices which are specialized ways to store matrix data when much of the matrix is empty.)

Coordinate Systems

All elements have the concept of a local coordinate system where they are aligned in a convenient orientation for deriving equations. When assembled into a finite element model, however, the element may be oriented in any orientation. Thus, a process of transformation is needed to transform the quantities involved in the constituent equations, such as force and displacement, from the local element system to the global coordinate system, and vice-versa. For that, we use a transformation matrix. In a previous post I demonstrated the basic concept of a transformation matrix.

Truss Element

The truss element is represented schematically and can be modeled as a spring: it may only take tension or compression. Each node has two DOF, x and y. The element coordinate system has its x-axis aligned with the element direction vector going from node i to node j. Quantities with respect to the local element coordinate system are indicated by the bar over the variable.

It is considered a discrete element as opposed to a continuum element which has its variables governed by differential equations.

With the element having constant properties A (area), E (elastic modulus), and an inferred length from the nodes, L, the element stiffness in the axial direction is:

\begin{equation*} k = \frac{AE}{L} \end{equation*}

Since the element may only take tension or compression, elemental y axis forces do not contribute to member stiffness. Thus, force equilibrium and force-displacement relations become:

\begin{equation*} \bar{f} = k\Delta x = \frac{AE}{L} (\bar{u}_{x,j} - \bar{u}_{x,i}) \end{equation*}

where \(\Delta x\) is the elongation of the bar, equal to \(\bar{u}_{x,j} - \bar{u}_{x,i}\)

Then, force equilibrium requires:

\begin{equation*} -\bar{f}_{x,i} = \bar{f}_{x,j} \end{equation*}

The local element stiffness equations are then as follows:

\begin{equation*} -\bar{f}_{x,i} = \frac{AE}{L} (\bar{u}_{x,j} - \bar{u}_{x,i}) \qquad \text{or} \qquad \bar{f}_{x,i} = \frac{AE}{L} (- \bar{u}_{x,j} + \bar{u}_{x,i}) \end{equation*}

\begin{equation*} \bar{f}_{x,j} = \frac{AE}{L} (\bar{u}_{x,j} - \bar{u}_{x,i}) \end{equation*}

Which can be combined into matrix form, \(\mathbf{\bar{F}} = \mathbf{\bar{K}}\mathbf{\bar{U}}\):

\begin{equation*} \begin{bmatrix} \bar{f}_{x,i} \\ \bar{f}_{y,i}\\ \bar{f}_{x,j}\\ \bar{f}_{y,j} \end{bmatrix} = \frac{AE}{L} \begin{bmatrix} 1 & 0 & -1 & 0 \\ 0 & 0 & 0 & 0\\-1 & - & 1 & 0\\ 0 & 0 & 0 & 0\end{bmatrix} \begin{bmatrix} \bar{u}_{x,i} \\ \bar{u}_{y,i}\\ \bar{u}_{x,j}\\ \bar{u}_{y,j} \end{bmatrix} \end{equation*}

The 4x4 matrix with the coefficient is the element stiffness matrix in the element coordinate system, and for an individual element in the context of a collection of elements is denoted as \(\mathbf{\bar{K}}^e\).

Transformation

Transformation is needed to convert element quantities in the local element coordinate system to those in the global element coordinate system so they may be appropriately combined into global stiffness equations. The position or orientation of the element is defined by the nodal coordinates.

\begin{equation*} \mathbf{\bar{u}_{x,i}} \end{equation*}

\begin{equation*} \mathbf{\bar{u}_{y,i}} \end{equation*}

Displacement transformations may be inferred from graphical analysis.

\begin{equation*} \bar{u}_{x,i} = u_{x,i}\cos\theta + u_{y,i}\sin\theta \end{equation*}

\begin{equation*} \bar{u}_{y,i} = -u_{x,i}\sin\theta + u_{y,i}\cos\theta \end{equation*}

The equations for node j are the same as for node i.

\begin{equation*} \bar{u}_{x,j} = u_{x,j}\cos\theta + u_{y,j}\sin\theta \end{equation*}

\begin{equation*} \bar{u}_{y,j} = u_{x,j}\sin\theta + u_{y,j}\cos\theta \end{equation*}

Putting all 4 equations into matrix form, and with the helpers of \(c=\cos\theta\) and \(s=\sin\theta\), we have:

\begin{equation*} \begin{bmatrix}\bar{u}_{x,i} \\ \bar{u}_{y,i} \\ \bar{u}_{x,j} \\ \bar{u}_{y,j}\end{bmatrix} = \begin{bmatrix} c & s & 0 & 0 \\ -s & c & 0 & 0 \\ 0 & 0 & c & s \\ 0 & 0 & -s & c\end{bmatrix} \begin{bmatrix} u_{x,i} \\ u_{y,i} \\ u_{x,j} \\ u_{y,j} \end{bmatrix} \end{equation*}

Force transformations are the same as for displacement:

\begin{equation*} \begin{bmatrix}\bar{f}_{x,i} \\ \bar{f}_{y,i} \\ \bar{f}_{x,j} \\ \bar{f}_{y,j}\end{bmatrix} = \begin{bmatrix} c & s & 0 & 0 \\ -s & c & 0 & 0 \\ 0 & 0 & c & s \\ 0 & 0 & -s & c\end{bmatrix} \begin{bmatrix} f_{x,i} \\ f_{y,i} \\ f_{x,j} \\ f_{y,j} \end{bmatrix} \end{equation*}

The 4x4 matrix used here is the transformation matrix and is denoted as \(\mathbf{T}^e\). Conversion of quantities from the global coordinate system to the element coordinate system is done by:

\begin{equation*} \mathbf{\bar{U}}^e = \mathbf{T}^e \mathbf{U}^e \end{equation*}

\begin{equation*} \mathbf{\bar{F}}^e = \mathbf{T}^e \mathbf{F}^e \end{equation*}

Global Equations

Generation of global equations is developed by first setting equal the equations for the local element on a force basis, which yields:

\begin{equation*} \mathbf{\bar{F}}^e = \mathbf{\bar{K}}^e \mathbf{\bar{U}}^e \end{equation*}

and is equal to:

\begin{equation*} \mathbf{T}^e\mathbf{F}^e = \mathbf{\bar{K}}^e \mathbf{T}^e\mathbf{U}^e \end{equation*}

Next, both sides are multiplied by \((\mathbf{T}^e)^{-1}\), which for this element type is also equal to the transpose, \((\mathbf{T}^e)^T\):

\begin{equation*} (\mathbf{T}^e)^T \mathbf{T}^e \mathbf{F}^e = (\mathbf{T}^e)^T \mathbf{\bar{K}}^e \mathbf{T}^e \mathbf{U}^e \end{equation*}

which becomes,

\begin{equation*} \mathbf{F}^e = (\mathbf{T}^e)^T \mathbf{\bar{K}}^e \mathbf{T}^e \mathbf{U}^e \end{equation*}

therefore, the element's stiffness matrix in global coordinates is:

\begin{equation*} \mathbf{K}^e = (\mathbf{T}^e)^T \mathbf{\bar{K}}^e \mathbf{T}^e \end{equation*}

References

Introduction to Finite Element Methods (ASEN 5007). University of Colorado at Boulder. http://kis.tu.kielce.pl/mo/COLORADO_FEM/colorado/Home.html.
J. N. Reddy, Ph.D. Introduction to the Finite Element Method, Fourth Edition. Analysis of Trusses, Chapter (McGraw-Hill Education: New York, Chicago, San Francisco, Athens, London, Madrid, Mexico City, Milan, New Delhi, Singapore, Sydney, Toronto, 2019, 2006, 1993, 1984). https://www.accessengineeringlibrary.com/content/book/9781259861901/toc-chapter/chapter6/section/section3

Experimenting with ANSYS ACT in Mechanical

2019-09-07T00:00:00-05:00

ANSYS ACT is the scripting API for various ANSYS products. It is available for Workbench, Mechanical, Fluent, and others. It uses Python 2 and in Mechanical it allows much of the standard click operations to be accessed programmatically.

Usage

In Mechanical, the ACT Console is a pane that allows for running and testing scripts. It is accessed by clicking the white rectangular icon next to the Help menu by default (in pre-tabbed interfaces - in ANSYS 2019R2, the program switched to a tabbed interface).

With the ACT Console open, you have more or less a standard Python interpreter. You issue commands in the command line (darkened area at the bottom), and see results in the area above it. The console features auto-completion and can be used interactively, especially while developing new scripts. New lines, such as with for loops, can be entered with SHIFT + ENTER.

There is a pane on the left which holds Snippets, which are simply files storing code for reuse. You can create your own snippets for actions that you want to remember or perform more than once. You do this by clicking on the Add Snippet button (left most icon in the snippet portion of the toolbar). Then, when you click on the snippet from the Bookmarks pane, the code is simply inserted into the command line and can be executed by pressing ENTER.

A collection of snippets can be grouped together and imported/exported. This might be useful if you or your company has a set of scripts that you use. To use this functionality, create a new group and give it a name. Drag your snippets into it. Then, in the ACT toolbar, export the snippets to an XML file. This exports all of the snippets, including the default ones that came loaded when you opened the console. These can easily be removed by editing the XML file after it is saved. In the XML file, find the group that has the name of your group, and delete everything else, not including the parent xml tags. For example, if I add the following snippet Snippet 1 and group My Snippets:

After exporting I find an xml file with the following:

<!--?xml version=\"1.0\" encoding=\"utf-8\"?-->
<model maxid=\"5\">
<root>
    <folder id=\"1\" label=\"Folder\">
    <bookmark id=\"2\" label=\"ExtAPI\">
    \t<!--[CDATA[ExtAPI.]]-->
    </bookmark>
    </folder>
    <folder id=\"4\" label=\"My Snippets\">
    <bookmark id=\"5\" label=\"Snippet 1\">
    \t<!--[CDATA[print Hello World!]]-->
    </bookmark>
    </folder>
</root>
</model>

In this case I will want to simply delete the <folder> item with the label=\"Folder\" attribute, since that is code not pertaining to my custom folder. ANSYS stores the actual code for the snippet in the bookmark field; in this case the code is print Hello World!.

API

An API is how operations and objects in Mechanical are retrieved and manipulated with code. The default global variable that gives access to all objects in Mechanical is ExtAPI. From this you can access all other objects using Python dot syntax. Listed below are some of the objects in Mechanical and their classes and access points. It is common to assign these to a variable so that they do not need to be fetched each time. For example:

solution = ExtAPI.DataModel.Project.Model.Analyses[0].Solution

Object	Access	Note
The Project	`ExtAPI.DataModel.Project`
List of Analyses	`ExtAPI.DataModel.Project.Model.Analyses`	This is list-like and indexable/loopable
Analysis working directory	`ExtAPI.DataModel.Project.Model.Analyses[0].WorkingDir`	Gets the working directory for the first analysis system (zeroth index)
Connections	`ExtAPI.DataModel.Project.Model.Connections`
Solution	`ExtAPI.DataModel.Project.Model.Analyses[0].Solution`	This is the solution object for the first analysis system (zeroth index)

Object	Class
Force Reaction Probe	`Ansys.ACT.Automation.Mechanical.Results.ProbeResults.ForceReaction`
Moment Reaction Probe	`Ansys.ACT.Automation.Mechanical.Results.ProbeResults.MomentReaction`
Beam Probe	`Ansys.ACT.Automation.Mechanical.Results.ProbeResults.BeamProbe`
Tree Group Folder	`Ansys.ACT.Automation.Mechanical.TreeGroupingFolder`

Change the Python directory to the `user_files` directory for a Project

Scripts that save out to a file might want to take advantage of the user_files directory. The user_files directory exists at the first level of the project files directory and is for storing user information pertaining to a Workbench project. I haven't found the path for this as a parameter in the API directly so the below is a way to obtain it from an analysis working directory. It splits the path at the Workbench project folder, so _files must not come before the Workbench folder in the path or it will return the wrong location.

from os import chdir
MECH_dir = ExtAPI.DataModel.Project.Model.Analyses[0].WorkingDir
user_dir = MECH_dir.split('_files')[0] + r'_files\user_files'
chdir(user_dir)

Usage Example: Results Exporting

One of the major limitations of Workbench / Mechanical is getting result probes out of Mechanical and into an external file (Excel, text file, etc.). If you only have a few result probes this is no problem - copy and paste will work fine. However, if you have a hundred, there is not an easy way to get all of the data and more importantly formatted as you like. Additionally, for a contact, you will likely want a Force Probe and a Moment Probe; these are two separate items in the Solution and you must export both and associate correctly with the contact they are referring to. With ACT, you can programmatically loop through these items and save them to a text file.

Beams

In this case you have some beams in your model defined under the Connections folder and you'd like to export the beam probes. If you've already created a result probe for them, you can retrieve and export them as follows:

solution = ExtAPI.DataModel.Project.Model.Analyses[0].Solution
beam_probes = filter(lambda item: item.GetType() == Ansys.ACT.Automation.Mechanical.Results.ProbeResults.BeamProbe, solution.Children)

f = open('Beam results.txt','w')
f.write('Beam Probes\n\n')
f.write('Name\tAxial Force\tTorque\tShear Force at I\tShear Force at J\tMoment at I\tMoment at J\n\n')

for bp in beam_probes:
    name = bp.BoundaryConditionSelection.Name
    f.write(name + '\t' +
        str(bp.AxialForce).split('[')[0] + '\t' +
        str(bp.Torque).split('[')[0] + '\t' +
        str(bp.ShearForceAtI).split('[')[0] + '\t' +
        str(bp.ShearForceAtJ).split('[')[0] + '\t' +
        str(bp.MomentAtI).split('[')[0] + '\t' +
        str(bp.MomentAtJ).split('[')[0] + '\n' )
f.close()

With the following tree, and after setting the working directory to the user_files directory, running the above code produces Beam results.txt:

Name    Axial Force Torque  Shear Force at I    Shear Force at J    Moment at I Moment at J

Bolt 1  23.464579153988097  -0.69336988094428165    95.214531366676013  95.214531366676013  12.945849648564687  11.227034167745025
Bolt 2  -23.464579153988097     -0.70081092496467057    104.8404773221031   104.8404773221031   14.025457881021863  12.521195678519947

This file is tab-delimited and the bolt names come from the name of the beam items in the Connections folder. Additionally, the unit is stripped from the result.

See full snippets on Github: https://github.com/robsiegwart/ANSYS-ACT-snippets.