Hypermesh Buckling Analysis
The lowest eigenvalue obtained from the analysis is the one associated with buckling. The critical load is the magnitude of the applied load times a factor of the critical eigenvalue.
Problem statement
When going through the steps hit return to continue and if nothing is said about a particular screen it’s because the settings in it don’t need to be changed. Also, you can name variables at your discretion, but I recommend you name them something that will help you get an idea of what they are. Let’s go.
When you start HyperMesh you will be prompted to enter a user profile. Make sure you change it to Standard2D as shown.
Create nodes
Geometry>nodes
In the case of the structure on the right the coordinates of the nodes are:
(0.0, 0.0, 0.0)
(0.0, 1.0, 0.0)
(1.5, 0.0, 0.0)
(1.5, 1.0, 0.0)
Create Material
Set Material Card
Check Elastic
E=2e11 (Elastic Modulus)
Nu=0.3 (Poisson’s ratio)
Create Property
Assign Material to Property
We will return to take care of this in a couple of steps
Create HyperBeam
This gives the beam a cross-section
1D>HyperBeam
Set the properties shown on the previous image. When you click create you will see the following:
Set dimensions (a) and (b) to 0.05 as defined in the problem statement. These are the cross-sectional width and height of the beam. When you’re done click “File>Exit” to go back.
Assign HyperBeam cross-section to the previously create property
Double clicking on “beamsec” will let you assign the previously created HyperBeam cross-section to the property.
You will notice that the values for (a) and (b) will be filled out and the options for other values will disappear. The other values are not used in the case of a square beam; they refer to dimensions of the different sections of I beams, etc.
The previous steps can be considered to be “housekeeping”. They defined the physical properties iof the beams that will be used to construct the model.
Now comes the fun part:
First we will connect each node with lines based on the design given in the problem statement. Then we will mesh the lines and assign them properties.
Connect each node with lines
Geom>lines
Connect each pair of nodes
Mesh and assign a property to the lines
Meshing means chopping up each line into a finite number of elements so you can analyze the properties of each one. (Hence the name Finite Element Analysis)
1D>line mesh
The element size determines the size of each chopped up line. In this case we will use 0.1 but you can make as large or as small as you want as long as its smaller than the section you’re meshing (duh).
element config: bar
This will turn the lines you previously created into bars. Bars have a cross section, are able to bend, and transmit loads. In contrast, if you were to make them rods, they would only be able to transmit loads, but not bend.
Double Click on property and assign to them the property you previously created.
Select each line and click mesh.
Don’t worry about this screen; hit return to continue.
Delete original nodes
Before we move on we need to delete the nodes we originally created. Nodes were created at those locations when we meshed the lines, and having redundant nodes will mess up the model.
Geom>temp nodes>clear all
Place Loads and Supports
Create>Load Collector
The card image for supports should be INITIAL_CONDITION and for loads it should be HISTORY.
Loads
Analysis>forces
Place the force on
In this case the force will be set to -2 in the Y direction. As mentioned at the beginning of the guide the critical load is a product of the load and eigenvectors. Because the problem statement shows 2P being applied, using -2 will mean that whatever the value of the lowest resulting eigenvalue will be the value of the critical load P. (you’ll see what I mean at the end)
Supports
Create another Load Collector (INITIAL_HISTORY) and this time do
Analysis>constraints
and place a hinge in its respective location.
dof1, dof2 and dof3 refer to translational motion in the x, y and z axes, respectively. dof4, dof5, and dof6 refer to rotational motion in the x, y, and z axes, respectively. Why not just name them x, y and z? I don’t know.
Anyway, in this case the problem statement indicates a ball hinge so we will only constrain dof1, dof2 and dof3 by checking them.
We are done with the model. The next step is to specify the variables that should be processed and output.
tools>Load Step Browser>New…>Create
Parameter>
check Name and Perturbation
NOTE: when going through each tab make sure to hit UPDATE or your changes won’t save
Analysis procedure>
Analysis type: buckle (duh)
Parameter>Eigen solver selects which solving method you want to use (does not matter in this case)
Dataline>number of eigenmodes: 5 works for now
Check, check
Output request>ODF file>New…
This will create an output file.
Checking Node and Element output will allow you to select which parameters of the nodes and elements you want to analyze. In this case we want to know the displacement U at the nodes and the stress S at each element. Remember to hit update.
Do the same thing for the Result and Data files (tabs on the left).
Export the model
Run the model through Abaqus
Open the Abaqus command and type
abaqus j=”filename”
Hit enter.
Abaqus will process the model and create a couple of files. You are interested in the INP (input) and DAT (data) files.
The DAT file contains the results for the analysis. If the analysis ran without errors you will find:
MODE NO EIGENVALUE
1 1.64650E+05
2 7.41579E+05
3 2.32366E+06
4 5.01343E+06
5 8.89534E+06
The analysis shows that the structure will buckle when P=1.64650E+05. That is under a load of (2)*(1.64650E+05)=3.293E+05 N
You can view how the structure will behave in the Abaqus Viewer. Simply open the software (a black cmd screen will appear for a couple of seconds, then the software will open) and open the .ODB file.
You can change how you want to view the model.
Result>Step/Frame
This will let you view the model under different eigenmodes.
I hope this helped. This is the first tutorial I make on the topic. I intend to improve the quality of the explanations as I make more.
