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

Modeling Plasticity & Performing a Restart Analysis in Abaqus

Last Updated:
(Published: )
This tutorial demonstrates how to include the effect of plasticity in a simulation using Abaqus, and also how to perform a restart analysis.

New Topics Covered

  • Understand how Abaqus uses plastic material properties
  • Read material data from an external file
  • Plot a stress vs plastic strain curve in Abaqus to visualize your own data
  • Understand increments and iterations and change the initial increment for a non-linear analysis
  • Understand restart analyses and request appropriate restart data
  • Create a new model to continue an analysis using restart data
  • Use the load  manager to enable/disable loads at a particular step
  • Change viewport annotation options to control the font size and style of legend, title block and state block
  • Create new visualization viewports and tile them
  • Use the frame selector tool to display specific frames
  • Render shell thickness

Overview

In this tutorial I analyze the plate from an earlier tutorial but this time the plate will deform plastically under the action of the load. which is loaded with concentrated forces at a few of its nodes. 

The plasticity behavior of the material is defined by the following stress vs strain curve:

We will request restart output for the load step. At the end of the load step we run a new job (which will be a restart analysis) where we will allow the plate to spring back so that it recovers its elastic deformation (although the plastic deformation will not be recovered). 

 

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. Open the model created for the elastic plate bending example of Chapter 10.
  2. Rename Plate Bending Model as Plastic Plate Bending Model
    • Right-click on Plate Bending Model in the Model Database
    • Choose Rename..
    • Change name to Plastic Plate Bending Model
  3. Modify the material
    • Expand the Materials container in the Model Tree
    • Right-click on AISI 1005 Steel
    • Choose Rename..
    • Change name to Steel
    • Right-click on AISI 1005 Steel
    • Choose Edit. The Edit Material window is displayed
    • Select Mechanical > Elasticity > Elastic. Change Poisson’s Ratio to 0.23
    • Select Mechanical >Plasticity>Plastic. Chang
    • Right-click in the Data table and choose Read from File. The Read Data from ASCII File window is displayed.
    • Set File  to plate_bending_steel_plasticity_data by clicking the Select button.
    • Set Start reading values into table row to 1
    • Set Start reading values into table column to 1
    • Set Base Feature Shape to Shell
    • Set Base Feature Type to Planar
    • Right-click in the table and choose Create XY Data…. The Create XY Data window is displayed.
    • Set Name to steel stress vs. plastic strain
    • Set Read X values from column to 2
    • Set Read Y values from column to 1
    • Set Approximate Size to 20
    • Click OK. You will enter Sketcher mode.
    • Switch to the Visualization module using the Module dropdown menu
    • Expand the XY Data container in the Results Tree
    • Double-click on steel stress vs. plastic strain in the Results tree. Aplot of the yield stress vs. plastic strain data is displayed
    • Click the XY Curve Options tool. The Curve Options window is displayed.
    • Set the Style to dashed using the dropdown menu.
    • Check Show symbol.
    • Change Symbol to another shape using the dropdown menu
    • Change Size to Large using the dropdown menu
    • Click Dismiss to close the window
  4. Edit the Step
    • Expand the Steps container in the Model Tree.
    • Double-click Load Step. The EditStep window is displayed
    • Switch to the Incrementation tab
    • Set Increment size to 0.1
  5. Edit Loads
    • Expand the Loads container in the Model Tree.
    • Double-click Concentrated Forces. The Edit Load window is displayed
    • Change CF3 to -270000.0 to apply a 270000.0 N force in downward (negative Y) direction
    • Click OK
  6. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to PlateJobPlastic
    • Set Source to Plastic Plate Bending Model
    • Select Plastic Plate Bending Model (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Job simulates the plastic bending of a plate
    • 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 PlateJobPlastic and choose Submit.
    • You will see a popup saying History output is not requested in the following steps: Load Step. OK to continue with job submission? Click Yes.
    • This will run the simulation. You will see the following messages in the message window: 
      Error in job PlateJobPlastic: THERE IS NO MATERIAL BY THE NAME AISI 1005 STEEL
      Error in job PlateJobPlastic: 90 elements have missing property definitions. The elements have been identified in error set ErrElemMissingSection
      Job PlateJobPlastic: Analysis Input File Processor aborted due to errors.
      Error in job PlateJobPlastic: Analysis Input File Processor exited with an error
      You will also see the word Aborted next to PlateJobPlastic in the Model Tree
  7. Edit Sections
    • Expand the Sections container in the Model tree
    • Double-click Concentrated Forces. The Edit Load window is displayed. You also see a message Section ‘Plate Section’ contains a reference to material ‘AISI 1005 Steel’, but that material no longer exists
    • Click Dismiss
    • Set Material to Steel using the drop down menu
    • Click OKto close the Edit Section window
  8. Resubmit the job
    • Right-click on PlateJobPlastic in the Jobs container of the Model tree and choose Submit.
    • You will see a popup saying Job files already exist for PlateJobPlastic. OK to overwrite? Click OK.
    • You will see a popup saying History output is not requested in the following steps: Load Step. OK to continue with job submission? Click Yes.
    • This will run the simulation. You will see the following messages in the message window: 
      The job input file "PlateJobPlastic.inp" has been submitted for analysis. 
      Job PlateJobPlastic: Analysis Input File Processor completed successfully
      Job PlateJobPlastic: Abaqus/Standard completed successfully
      Job PlateJobPlastic completed successfully
  9. Plot contour and change font of legend, title block and state block
    • Right-click on PlateJobPlastic (Completed) in the Model Database. Choose Results. The viewport changes to the Visualization module.
    • In the toolbar choose Plot Contours on Deformed Shape tool to plot the Mises stress contours on the plate
    • In the menu bar click on Viewport > Viewport Annotation Options
    • Switch to the Legend tab
    • Click Set Font. The Select Font window is displayed.
    • Set Size to 14 using the dropdown menu
    • For Apply To check Legend
    • Click Ok. The font size of the legend is now 14.
    • Switch to the Title Block tab
    • Click Set Font. The Select Font window is displayed.
    • Set Font to Times New Roman using the dropdown menu
    • Set Size to 14 using the dropdown menu
    • For Style check Italic
    • For Apply To check Title block and State block
    • Click OK
  10. Request Field Outputs
    • Switch to the Step module using the Module dropdown menu
    • Using the menu bar click on Output > Restart Requests... The Edit Restart Requests window is displayed.
    • In the Frequency column, set the frequency to 1 for Load Step
    • Check Overlay
    • Click OK
  11. Resubmit the job
    • Right-click on PlateJobPlastic in the Jobs container of the Model tree and choose Submit.
    • You will see a popup saying Job files already exist for PlateJobPlastic. OK to overwrite? Click OK.
    • You will see a popup saying History output is not requested in the following steps: Load Step. OK to continue with job submission? Click Yes.
    • This will run the simulation. You will see the following messages in the message window: 
      The job input file "PlateJobPlastic.inp" has been submitted for analysis. 
      Job PlateJobPlastic: Analysis Input File Processor completed successfully
      Job PlateJobPlastic: Abaqus/Standard completed successfully
      Job PlateJobPlastic completed successfully
  12. Check the Abaqus work directory – it is C:\Temp by default – for the presence of a restart file PlateJobPlastic.res
  13. Copy the model to create a restart model
    • Right click on Plastic Plate Bending Model in the Model tree.
    • Choose Copy Model.. The Copy Model dialog box is displayed
    • Set Copy Plastic Plate Bending Model to: to Plate Springback Model
    • Click OK. A new model Plate Springback Model is displayed in the Model tree
    • Right click on Plate Springback Model.
    • Choose Edit Attributes.. The Edit Model Attributes window is displayed
    • In the Restart tab check Read data from joband type in PlateJobPlastic
    • Set Step name to Load Step
    • Click Ok..
  14. Add a new step
    • Double-click on Steps container in the Model Tree. The Create Step window is displayed
    • Set Name to Springback
    • Set Insert New Step After to Load Step
    • Set Procedure Type to General > Static, General
    • Click Continue.. The Edit Step window is displayed
    • In the Basic tab, set Description to Remove load and allow elastic springback.
    • Set Time period to 1
    • Switch to the Incrementation tab
    • Set Initial Increment size to 0.1
    • Click OK.
  15. Deactivate the load in the Springback step
    • Right click on Loads in the Model tree.
    • Choose Manager.. The Load Manager dialog box is displayed
    • Click Propagated in the Springback step. The word Propagated changes to Inactive
    • Click Deactivate
    • Click Dismiss.
  16. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to PlateSpringbackJob
    • Set Source to Plate Springback Model
    • Select Plastic Plate Bending Model (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Job allows elastic springback
    • Set Job Type to Restart.
    • Leave all other options at defaults
    • Click OK
    • Expand the Jobs container in the Model Database
    • Right-click on PlateSpringbackJob and choose Submit.
    • You will see a popup saying History output is not requested in the following steps: Load Step. OK to continue with job submission? Click Yes.
    • This will run the simulation. You will see the following messages in the message window:
      The job input file "PlateJobPlastic.inp" has been submitted for analysis. 
      Job PlateSpringbackJob: Analysis Input File Processor completed successfully
      Job PlateSpringbackJob: Abaqus/Standard completed successfully
      Job PlateSpringbackJob completed successfully
  17. Plot contour
    • Right-click on PlateSpringbackJob (Completed) in the Model Tree. Choose Results. The viewport changes to the Visualization module.
    • In the toolbar choose Plot Contours on Deformed Shape tool to plot the Mises stress contours on the plate
    • In the menu bar click on Viewport > Create. A new viewport is created. It may be hidden behind the current viewport if you cannot seen
    • In the menu bar click on Viewport > Tile Vertically. The two viewports are placed side by side. The new viewport has the same contents as the old one.
    • Click the titlebar of Viewport 1 to make it the active viewport.
    • Right click on Output Databases in the Results tree and choose Open
    • Choose PlateJobPlastic.odb from the Open Database browse window. The results of the original analysis are displayed in the viewport.
    • In the toolbar choose Plot Contours on Deformed Shape tool to plot the Mises stress contours on the plate
    • Click the titlebar of Viewport 2 to make it the active viewport.
    • Use the ODB dropdown menu (above the viewport) to ensure that the ODB is set to PlateSpringbackJob.odb
    • Again click the titlebar of Viewport 1 to make it the active viewport.
    • Click the Frame Selector tool. You see the Frame Selector dialog box
    • Set the frame to the last frame (frame 14) of the Load step
    • Close the Frame Selector tool by clicking the red x at the top right corner of the dialog box
    • Again click the titlebar of Viewport 2 to make it the active viewport.
    • Click the Frame Selector tool. You see the Frame Selector dialog box
    • Set the frame to the first frame (frame 0) of the Springback step
    • Compare the contour plots and the legends. They should be identical.
    • Click the titlebar of Viewport 1 to make it the active viewport
    • Change the primary field variable to UT (translations and rotations) U3 using the field output toolbar. The displacement contour is displayed on the plate
    • Click the titlebar of Viewport 2 to make it the active viewport
    • Change the primary field variable to UT (translations and rotations) U3 using the field output toolbar. The displacement contour is displayed on the plate
    • Compare the contour plots and the legends. They should be identical
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
Hi Gautam! Thanks for your video! I want to ask can I restart the job which is already restarted from a previous job. For example, I restarted the job to add load, but I found the additional load is not enough; I want to add more load.
Like
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.