This article is part of a series titled Abaqus FEA Tutorial Series

Static Analysis of a Truss using Abaqus

Last Updated:
(Published: )
This tutorial demonstrates how to perform a static analysis on a 2 dimensional truss structure using Abaqus FEA.

New Topics Covered

  • How to work in 2D
  • Create truss members in the sketcher using the Create Lines: Connected tool
  • Create sections of type truss and specify cross sectional areas
  • Use truss elements (with pin joints)
  • Use concentrated force loads
  • Allow multiple plot states (both deformed and undeformed plots overlaid)
  • Display node labels using Common Plot Options -> Show Node Labels
  • Display field output as color contours

Overview

In this tutorial I analyze a 2D truss structure which is loaded with concentrated forces at a few of its nodes. 

Truss structures are designed to carry axial loads (tensile and compressive) without any bending, and the nodes of a truss structure are pin joints meaning that they only transfer forces and not moments. Therefore I model the truss using wire features and mesh the structure using truss elements which are internally formulated only carry axial loads and deform in the form of axial stretching and are assumed to be pin jointed at their nodes.  

Procedure

a. Overview

B. Part 1

C. Part 2

Procedure In Text Form

This is a text version of the steps followed in the videos above. (To understand why these steps were followed please watch the videos with the sound turned on).

  1. Rename Model-1 to Truss Structure
    • Right-click on Model-1 in Model Database
    • Choose Rename..
    • Change name to Truss Structure
  2. Create the part
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Truss
    • Set Modeling Space to 2D Planar
    • Set Type to Deformable
    • Set Base Feature to Wire
    • Set Approximate Size to 10
    • Click OK. You will enter Sketcher mode.
  3. Sketch the truss
    • Use the Create Lines:Connectedtool to draw the profile of the truss
    • Split the lines using the Split tool
    • Use Add Constraints > Equal Length tool to set the lengths of the required truss elements to be equal
    • Use the Add Dimension tool to set the length of the horizontal elements to 2 m and the length of the vertical elements to 1.5 m.
    • Click Done to exit the sketcher.
  4. Create the material
    • Double-click on Materials in the Model Database. Edit Material window is displayed
    • Set Name to AISI 1005 Steel
    • Select General > Density. Set Mass Density to 7872 (which is 7.872 g/cc)
    • Select Mechanical > Elasticity > Elastic. Set Young’s Modulus to 200E9 (which is 200 GPa) and Poisson’s Ratio to 0.29.
  5. Assign sections
    • Double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Truss Section
    • Set Category to Beam
    • Set Type to Truss
    • Click Continue… The Edit Section window is displayed.
    • In the Basic tab, set Material to the AISI 1005 Steel which was defined in the create material step.
    • Set Cross-sectional Area to 3.14E-4
    • Click OK.
  6. Assign the section to the truss
    • Expand the Parts container in the Model Database. Expand the part Truss.
    • Double-click on Section Assignments
    • You see the message Select the regions to be assigned a section displayed below the viewport
    • Click and drag with the mouse to select the entire truss.
    • Click Done. The Edit Section Assignment window is displayed.
    • Set Section to Truss Section.
    • Click OK.
    • Click Done.
  7. Create the Assembly
    • Double-click on Assembly in the Model Database. The viewport changes to the Assembly Module.
    • Expand the Assembly container.
    • Double-click on Instances. The Create Instance window is displayed.
    • Set Parts to Truss
    • Set Instance Type to Dependent (mesh on part)
    • Click OK.
  8. Create Steps
    • Double-click on Steps in the Model Database. The Create Step window is displayed.
    • Set Name to Loading Step
    • Set Insert New Step After to Initial
    • Set Procedure Type to General > Static, General
    • Click Continue.. The Edit Step window is displayed
    • In the Basic tab, set Description to Loads are applied to the truss in this step.
    • Click OK.
  9. Request Field Outputs
    • Expand the Field Output Requests container in the Model Database.
    • Right-click on F-Output-1 and choose Rename…
    • Change the name to Selected Field Outputs
    • Double-click on Selected Field Outputs in the Model Database. The Edit Field Output Request window is displayed.
    • Select the desired variables by checking them off in the Output Variables list. The variables we want are S (stress components and invariants), U (translations and rotations), RF (reaction forces and moments), and CF (concentrated forces and moments). Uncheck the rest. You will notice that the text box above the output variable list displays S,U,RF,CF
    • Click OK.
  10. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to Force1
    • Set Step to Loading Step
    • Set Category to Mechanical
    • Set Type for Selected Step to Concentrated Force
    • Click Continue…
    • You see the message Select points for the load displayed below the viewport
    • Select the upper left node by clicking on it
    • Click Done. The Edit Load window is displayed
    • Set CF2 to -3000 to apply a 3000 N force in downward (negative Y) direction
    • Click OK
    • You will see the force displayed with an arrow in the viewport on the selected node
    • Repeat steps a-l two more times, once each for the upper middle and upper right node. Name the forces Force2 and Force3, and set them to -5000 and -6000 respectively.
  11. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Pin1
    • Set Step to Initial
    • Set Category to Mechanical
    • Set Types for Selected Step to Displacement/Rotation
    • Click Continue…
    • You see the message Select regions for the boundary condition displayed below the viewport
    • Select the two nodes on the extreme left. You can press the “Shift” key on your keyboard  to select both at the same time.
    • Click Done. The Edit Boundary Condition window is displayed.
    • Check off U1 and U2. This will create a pin joint which does not allow translation but permits rotation.
    • Click OK.
  12. Create the mesh
    • Expand the Parts container in the Model Database.
    • Expand Truss
    • Double-click on Mesh (Empty). The viewport window changes to the Mesh module and the tools in the toolbar are now meshing tools.
    • Using the menu bar click on Mesh > Element Type …
    • You see the message Select the regions to be assigned element types displayed below the viewport
    • Click and drag using your mouse to select the entire truss.
    • Click Done. The Element Type window is displayed.
    • Set Element Library to Standard
    • Set Geometric Order to Linear
    • Set Family to Truss
    • You will notice the message T2D2: A 2-node linear 2-D truss
    • Click OK
    • Click Done
    • Using the menu bar lick on Seed > Edge by Number
    • You see the message Select the regions to be assigned local seeds displayed below the viewport
    • Click and drag using your mouse to select the entire truss
    • Click Done.
    • You see the prompt Number of elements along the edges displayed below the viewport.
    • Set it to 1 and press the “Enter” key on your keyboard
    • Click Done
    • Using the menu bar click on Mesh > Part
    • You see the prompt OK to mesh the part? displayed below the viewport
    • Click Yes
  13. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to TrussAnalysisJob
    • Set Source to Model
    • Select Truss Structure (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Analysis of truss under concentrated loads
    • Set Job Type to Full Analysis.
    • Leave all other options at defaults
    • Click OK
    • Expand theJobs container in the Model Database
    • Right-click on TrussAnalysisJob and choose Submit. This will run the simulation. You will see the following messages in the message window: 
      The job input file "TrussAnalysisJob.inp" has been submitted for analysis. 
      Job TrussAnalysisJob: Analysis Input File Processor completed successfully
      Job TrussAnalysisJob: Abaqus/Standard completed successfully
      Job TrussAnalysisJob completed successfully
  14. Plot results deformed and undeformed
    • Right-click on TrussAnalysisJob (Completed) in the Model Database. Choose Results.The viewport changes to the Visualization module.
    • In the toolbar click the Plot Undeformed Shape tool. The truss is displayed in its undeformed state.
    • In the toolbar click the Plot Deformed Shape tool. The truss is displayed in its deformed state.
    • In the toolbar click the Allow Multiple Plot States tool. Then click the Plot Undeformed Shape tool. Both undeformed and deformed shapes are now visible superimposed on one another.
    • Click again on the Allow Multiple Plot States tool to disallow this feature. Click on Plot Deformed Shape to have the deformed state displayed once again in the viewport.
    • In the toolbar click the Common Options tool. The Common Plot Options window is displayed.
    • In the Labels tab check Show node labels
    • Click OK. The nodes are now numbered on the truss in the viewport.
  15. Plot Field Outputs
    • Using the menu bar click on Result > Field Output... The Field Output window is displayed.
    • In the Output Variable list select U which has the description Spatial displacement at nodes. In the Invariant list Magnitude is displayed. In the Components list U1 and U2 are displayed
    • In the Invariant list select Magnitude. Click Apply. You might see the Select Plot State window with the message The field output variable has been set, but it will not affect the current Display Group instance unless a different plot state is selected below. For the Plot state select Contour and click OK.
    • Click OK to close the Field Output window. You notice in the viewport a color contour has been applied on the truss with a legend indicating the U magnitude.
    • Once again, using the menu bar click on Result > Field Output... The Field Output window is displayed.
    • In the Output Variable list select U which has the description Spatial displacement at nodes.
    • In the Component list select U1.
    • Click OK. The visualization updates to display U1 which is displacement in the X direction.
This article is part of a series titled Abaqus FEA Tutorial Series
Did you find this article interesting?
Get notified when Gautam writes more articles:
Comments
This website uses cookies to deliver services, improve usability, and measure performance. By continuing to use this site you opt-in to receive these cookies. You may disable some of them on the Cookie Settings page. You also acknowledge that you have read and understand our Cookie Policy, Privacy Policy, and Terms of Service.