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

Analysis of a Planar Shell (Plate) using Abaqus

Last Updated:
(Published: )
This tutorial demonstrates how to perform an analysis of a shell structure

New topics covered

  • Work in 3D with a planar shell
  • Create sections of type ‘shell’, specify section integration properties and assign shell thickness, and understand concepts such as Simpson and Gauss thickness integration rules
  • Understand and define shell offset when assigning sections
  • Decide if the NLGEOM (non-linear geometry) option should be used and turn it on/off as required
  • Delete history outputs
  • Create partitions for the purpose of generating selectable nodess
  • Show element labels on meshed model
  • Change the sort variable and sort order in the report profile
  • View/Change the Work Directory

Overview

In this tutorial I analyze a flat plate which bends due to the application of concentrated forces. 

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 Plate Bending Model
    • Right-click on Model-1 in the Model Database
    • Choose Rename..
    • Change name to Blate Bending Model
  2. Create the part
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Plate
    • Set Modeling Space to 3D 
    • Set Type to Deformable
    • Set Base Feature Shape to Shell
    • Set Base Feature Type to Planar
    • Set Approximate Size to 20
    • Click OK. You will enter Sketcher mode.
  3. Sketch the plate
    • Use the Create Lines:Rectangle (4 lines)  tool to draw the profile of the plate. Start at the origin and drag to the top and left so that the rectangle has positive X and Y coordinates.
    • Use the Add Dimension tool to set the length of the horizontal elements to 5 m and the length of the vertical elements to 3 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. Create sections
    • Double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Plate Section
    • Set Category to Shell
    • Set Type to Homogeneous
    • Click Continue… The Edit Section window is displayed.
    • In the Basic tab , set Section integration to During Analysis
    • Set Shell thickness Value to 0.1
    • Set Material to the AISI 1005 Steel which was defined in the material creation step.
    • Set Thickness integration rule to Simpson
    • Click OK.
  6. Assign the section to the plate
    • Expand the Parts container in the Model Database. Expand the part Plate.
    • 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 plate.
    • Click Done. The Edit Section Assignment window is displayed.
    • Set Section to Plate Section.
    • Set Shell Offset Definition to Middle surface.
    • Click OK.
  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 Plate
    • 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 Load 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 Apply concentrated forces in this step.
    • Set Time period to 1
    • Set Nlgeom to On
    • 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 Output Stresses and Displacements
    • Double-click on Output Stresses and Displacements 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) and U (translations and rotations). Uncheck the rest. You will notice that the text box above the output variable list displays S,U
    • Click OK.
  10. Delete History Outputs
    • Expand the History Output Requests container in the Model Database.
    • Right-click on H-Output-1 and choose Delete…
    • You see a prompt OK to delete “H-Output-1”? Click Yes.
  11. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Fix Edge
    • 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 left edge of the plate.
    • Click Done. The Edit Boundary Condition window is displayed.
    • Check off U1, U2, U3, UR1, UR2 and UR3. This will fix the edge and not allow translation or rotation.
    • Click OK.
  12. Partition the plate to create points for the concentrated loads
    • Expand the Parts container in the model tree.
    • Double-click the part Plate. The viewport changes to the Part module and plate part.
    • Click the Create Datum Point: Enter coordinates tool. You see the prompt Coordinates for datum point (X, Y, Z): below the viewport
    • Type in the coordinates 0.0, 2.0, 0.0 and press the “Enter” key on your keyboard. You see a datum point appear on the left edge of the plate in the viewport. You again see the prompt Coordinates for datum point (X, Y, Z): below the viewport
    • Type in the coordinates 0.0, 1.0, 0.0 and press the “Enter” key on your keyboard.. You see another datum point appear on the left edge of the plate in the viewport.
    • Similarly proceed to enter in the coordinates of the next 2 datum points which are 5.0, 2.0, 0.0 and 5.0, 1.0, 0.0 respectively. There are now 4 datum points, 2 on the left edge and 2 on the right edge of the plate.
    • Click the Partition Face: Use Shortest Path Between 2 Points tool. You see the message Select a start point below the viewport
    • Click on the top left datum point (whose coordinates are 0.0, 2.0, 0.0). You see the message Select an end point below the viewport.
    • Click on the top right datum point (whose coordinates are 5.0, 2.0, 0.0). You see the message Partition definition complete below the viewport
    • Click on the Create Partition button. The partition is displayed in the viewport.
    • You see the prompt Select the faces to partition below the viewport. Use the drop down to set it to individually.
    • Hover the mouse over the lower half of the plate (below the partition line). It will light up as you are hoving over it. Click it to select it.
    • Click Done. You see the message Select a start point below the viewport
    • Click on the bottom left datum point (whose coordinates are 0.0, 1.0, 0.0). You see the message Select an end point below the viewport
    • Click on the bottom right datum point (whose coordinates are 5.0, 1.0, 0.0). You see the message Partition definition complete below the viewport
    • Click on the Create Partition button. The second partition is displayed in the viewport and the plate now consists of 3 different partitions.
    • Click Done
  13. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to Concentrated Forces
    • Set Step to Load Step
    • Set Category to Mechanical
    • Set Type for Selected Step to Concentrated force
    • Click Continue…
    • You see the message Select points for the loaddisplayed below the viewport
    • Select the two points on the right edge where the partition line meets the edge. The reason for creating the partitions was to be able to select these two points. Hold the “Shift” key on your keyboard to select both points.
    • Click Done. The Edit Load window is displayed
    • Set CF3 to -7000.0 to apply a 7000 N force in downward (negative Y) direction
    • Click OK
    • You will see the forces displayed with an arrows in the viewport on the selected points although you may need to rotate the view to see them clearly
  14. Create the mesh
    • Expand the Parts container in the Model Database.
    • Expand Plate
    • 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 plate.
    • Click Done. The Element Type window is displayed.
    • Set Element Library to Standard
    • Set Geometric Order to Quadratic
    • Set Family to Shell
    • You will notice the message S8R: An 8-node doubly curved thick shell, reduced integration
    • 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 on the 6 vertical edges (3 on left edge and 3 on right edge). You will need to press the ‘Shift’ key on your keyboard to select all 6 of them
    • Click Done. You see the prompt Number of elements along the edges displayed below the viewport
    • Set it to 3 and press the “Enter” key on your keyboard.
    • Again you see the message Select the regions to be assigned local seeds displayed below the viewport
    • Click on the 4 horizontal edges (top edge, bottom edge and 2 partition lines). You will need to press the ‘Shift’ key on your keyboard to select all 4 of them
    • Click Done. You see the prompt Number of elements along the edges displayed below the viewport
    • Set it to 10 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. The meshed plate appears in the viewport.
  15. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to PlateJob
    • Set Source to Model
    • Select Plate Bending Model (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Job simulates the 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 PlateJob 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 "PlateJob.inp" has been submitted for analysis. 
      Job PlateJob: Analysis Input File Processor completed successfully
      Job PlateJob: Abaqus/Standard completed successfully
      Job PlateJob completed successfully
  16. Show element labels and plot contours
    • Right-click on PlateJob (Completed) in the Model Database. Choose Results. The viewport changes to the Visualization module.
    • In the toolbar click the Plot Undeformed Shape tool. The plate is displayed in its undeformed state.
    • In the toolbar click the Common Options tool. The Common Plot Options window is displayed.
    • In the Labels tab check Show element labels
    • Click OK. The elements are now numbered on the truss in the viewport.
    • In the toolbar click the Plot Contours on Deformed Shape tool. A color contour of S. Mises stresses is plotted over the plate
  17. Report Field Outputs
    • Using the menu bar click on Report> Field Output... The Report Field Output window is displayed.
    • In the Variable tab, set the Output Variables Position to Integration Point.
    • In the list you see S: Stress components. Click the arrow next to it to expand the list. Select Mises by checking it off
    • In the Setup tab, set the File Name to platestresses.rpt.
    • Uncheck the Append to file option
    • Set Sort by to S.Mises using the dropdown
    • Set it to Descending
    • For Write check Field output, Column totals and column min/max.
    • Click OK to close the Field Output window. In the message area you see The field output report was appended to file "platestresses.rpt".
    • You can now use windows explorer to navigate to the Abaqus temporary files directory. Open platestresses.rpt using WordPad. You will find that the stresses have been tabulated with element labels. In addition the maximum and minimum stresses are displayed at the bottom of the report.
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.