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

Dynamic Analysis of a Truss using Abaqus Explicit

Last Updated:
(Published: )
This tutorial demonstrates how to perform a transient dynamic analysis using the Abaqus Explicit solver. The model used is a 2 dimensional truss structure .

New topics covered

  • Create sets in the assembly
  • Change step time period and tell Abaqus to include non-linear geometry effects (NLGEOM)
  • Use history output requests specifying the domain and frequency of history outputs
  • Specify point of application of loads using sets
  • Plot history outputs
  • Save XY data of history output plots
  • Write XY data to a report
  • Display Field Output as color contours

Overview

In this tutorial I analyze a 2D truss structure which is dynamically loaded with concentrated forces for a short duration. 

This setup is similar to the previous one except that there is only one concentrated force load which is applied for a very short duration and I am interested in the dynamic reaction of the structure to this load.

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: Connected  tool 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 material creation 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. Identify Sets
    • Expand the Assembly container in the Model Database.
    • Double-click on Sets. The Create Set window is displayed.
    • Set Name to force point set
    • Click Continue…
    • You see the message Select the geometry for the set displayed below the viewport
    • Select the node on which the force will be applied by clicking on it
    • Click Done.
    • Once again double-click on Sets. The Create Set window is displayed.
    • Set Name to end point set
    • Click Continue…
    • You see the message Select the geometry for the set displayed below the viewport
    • Select the node on the extreme right
    • Click Done
  9. 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 >Dynamic, Explicit
    • Click Continue.. The Edit Step window is displayed
    • In the Basic tab, set Description to Loads are applied to the trussfor 0.01s in this step.
    • Set Time period to 0.01
    • Click OK.
  10. Request History Outputs
    • Expand the History Output Requests container in the Model Database
    • Right-click on H-Output-1 and choose Rename…
    • Change the name to Force Point Output
    • Double-click on Force Point Output in the Model Database. The Edit History Output Request window is displayed
    • Set Domain to Set. A new dropdown list appears next to it.
    • Choose force point set from this list
    • Set Frequency to Every n time increments.
    • Set n: to 1
    • Select the desired variables by checking them off in the Output Variables list. The variable we want is UT (translations) from the Displacement/Velocity/Acceleration group. Uncheck the rest. You will notice that the text box above the output variable list displays UT
    • Click OK
    • We need to create the second history output request. Double-click on History Output Requests in the Model Database. The Create History window is displayed
    • Set Name to End Point Output
    • Set Step to Loading Step
    • Click Continue… The Edit History Output Request window is displayed
    • Set Domain to Set. A new dropdown list appears next to it.
    • Choose end point set from this list.
    • Set Frequency to Every n time increments
    • Set n: to 1
    • Select the desired variables by checking them off in the Output Variables list. The variable we want is UT (translations) from the Displacement/Velocity/Acceleration group. Uncheck the rest. You will notice that the text box above the output variable list displays UT
    • Click OK
  11. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to ForcePulse
    • 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
    • We could select the required node by clicking on it. However we have already created a set for it. So click on the button Sets at the bottom of the viewport. The Region Selection window is displayed
    • Choose force point set from the list. You may check off Highlight selections in viewport if you wish to see the selected node light up
    • Click Continue... The Edit Load window is displayed
    • Set CF2 to -6000 to apply a 6000 N force in downward (negative Y) direction. Notice that Amplitude is set to (Instantaneous) although you cannot change it here.
    • Click OK
    • You will see the force displayed with an arrow in the viewport on the selected node
  12. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Pin
    • Set Step to Initial
    • Set Category to Mechanical
    • Set Types for Selected Step to Displacement/Rotation
    • Click Continue…
    • Since you earlier selected vertices in the viewport by clicking the Sets button, you will now see the Region Selection window asking you to choose the set on which to apply boundary conditions. You also see the message Select a region from the dialog at the bottom of the viewport. However we do not wish to apply it on either force point set or end point set. Notice also the button Select in Viewport at the bottom right of the viewport. Click it. You now 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.
  13. 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 lick on Mesh > Part
    • You see the prompt OK to mesh the part? displayed below the viewport
    • Click Yes
  14. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to TrussExplicitAnalysisJob
    • 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 a pulse load
    • Set Job Type to Full Analysis.
    • Leave all other options at defaults
    • Click OK
    • Expand the Jobs container in the Model Database
    • Right-click on TrussExplicitAnalysisJob and choose Submit. This will run the simulation. You will see the following messages in the message window: 
      The job input file "TrussExplicitAnalysisJob.inp" has been submitted for analysis. 
      Job TrussExplicitAnalysisJob: Analysis Input File Processor completed successfully
      Job TrussExplicitAnalysisJob: Abaqus/Standard completed successfully
      Job TrussExplicitAnalysisJob completed successfully
  15. Plot History Outputs
    • Using the menu bar click on Result >History Output... The History Output window is displayed.
    • In the Output Variable list select Spatial displacement: U2 at Node 4 in NSET END POINT SET
    • Click the Plot button. A plot of the vertical displacement of the node at the extreme right of the truss is displayed in the viewport.
    • Click the Save As… button. The Save XY Data As window is displayed.
    • Set Name to Data for end point
    • Click OK
    • In the Output Variable list select Spatial displacement: U2 at Node 4 in NSET FORCE POINT SET
    • Click the Plot button. A plot of the vertical displacement of the node at which the force was applied is displayed in the viewport.
    • Click the Save As… button. The Save XY Data As window is displayed.
    • Set Name to Data for force point
    • Click the Dismiss button
    • Using the menu bar click on Report>XY... The Report XY Data window is displayed
    • In the XY Data tab, make sure Select from: is set to All XY data. Data for end point and Data for force point should be displayed in the list. However sometimes due to a bug in Abaqus the list may appear empty and needs to be refreshed. To remedy this change Select from: to XY plot in current view and then back to All XY data. You should now see our XY data sets in the list.
    • Click Data for end point to make sure it is selected.
    • Click on the Setup tab.
    • In the File section, set Name to end_point_xydata_output.txt.
    • Uncheck Append to file.
    • In the Data section, for Write: check XY data, Columns totals and Column min/max
    • Switch back to XY Data tab
    • Make sure Data for end point is selected.
    • Click Apply. The file end_point_xydata_output.txt will be written to your Abaqus working directory.
    • Click Data for force point to make sure it is selected.
    • Click on the Setup tab.
    • In the File section, set Name to force_point_xydata_output.txt.
    • Uncheck Append to file.
    • In the Data section, for Write: check XY data, Columns totals and Column min/max
    • Switch back to XY Data tab
    • Make sure Data for end point is selected.
    • Click Apply. The file force_point_xydata_output.txt will be written to your Abaqus working directory.
    • Click Cancel to close the Report XY Data window.

 

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.