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

Assemblies and Tie Constraints in Abaqus

Last Updated:
(Published: )
In this tutorial an analysis is performed on a sandwich structure to demonstrate how to assemble and tie various parts in Abaqus FEA.

New Topics Covered

  • Using the pattern tool to create linear patterns in the sketcher
  • Assembling parts together
  • Understand tie constraints and their use in simulations

Overview

In this tutorial I analyze a sandwich structure consisting of two plates and a honeycomb. The three parts are tied together where they meet.

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 Sandwich Structure
    • Right-click on Model-1 in Model Database
    • Choose Rename..
    • Change name to Sandwich Structure
  2. Create the Top Layer
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Top Layer
    • Set Modeling Space to 3D 
    • Set Type to Deformable
    • Set Base Feature Shape to Solid
    • Set Base Feature Type to Extrusion
    • Set Approximate Size to 20
    • Click OK. You will enter the sketcher mode.
    • Use the Create Lines:Rectangle (4 lines)  tool to draw the profile of the plank
    • Use the Add Dimension tool to set the width to 0.2 m and the thickness to 0.03 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Depth to 0.8
    • Click OK.
  3. Create the Core Layer
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Core Layer
    • Set Modeling Space to 3D 
    • Set Type to Deformable
    • Set Base Feature Shape to Solid
    • Set Base Feature Type to Extrusion
    • Set Approximate Size to 20
    • Click OK. You will enter Sketcher mode.
    • Use the Create Lines: Rectangle (4 lines)  tool to draw the profile of the plank
    • Use the Add Dimension tool to set the width to 0.2 m and the thickness to 0.08 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Depth to 0.8
    • Click OK.
    • Click Create Cut: Extrude tool.
    • You see the message Select a plane for the extruded cut displayed below the viewport
    • Select the top face of the core layer.
    • You see the message Select an edge or axis that will appear vertical and on the right displayed below the viewport
    • Select the left edge of the core layer block. You will enter the Sketcher.
    • Use the Create Lines: Rectangle (4 lines) tool to draw 6 rectangles that will be cut out of the core.
    • Use the Add Dimension tool on each of these rectangles to set the x-dimension to 0.087 m and the y-dimension to 0.12.
    • Click Done to exit the sketcher. The Edit Cut Extrusion window is displayed.
    • Use the Add Dimension tool to set the width to 0.2 m and the thickness to 0.08 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Type to Through All.
    • If Extrude Direction is not through the block (see arrow) then click Flip
    • Click OK.
  4. Create the Bottom Layer
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Bottom Layer
    • Set Modeling Space to 3D 
    • Set Type to Deformable
    • Set Base Feature Shape to Solid
    • Set Base Feature Type to Extrusion
    • Set Approximate Size to 20
    • Click OK. You will enter Sketcher mode.
    • Use the Create Lines:Rectangle (4 lines) tool to draw the profile of the plank
    • Use the Add Dimension tool to set the width to 0.2 m and the thickness to 0.03 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Depth to 0.8
    • Click OK.
  5. 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 7800 (which is 7.800 g/cc)
    • Select Mechanical > Elasticity > Elastic. Set Young’s Modulus to 200E9 (which is 200 GPa) and Poisson’s Ratio to 0.29.
    • Click OK.
  6. Create 3 sections
    • Double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Top Layer Section
    • Set Category to Solid
    • Set Type to Homogeneous
    • 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.
    • Click OK.
    • Again double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Top Layer Section
    • Set Category to Solid
    • Set Type to Homogeneous
    • 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.
    • Repeat steps a thru m to create two more sections Core Layer Section and Bottom Layer Section
    • Click OK.
  7. Assign the sections to the parts
    • Expand the Parts container in the Model Database. Expand the part Top Layer.
    • 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 top layer.
    • Click Done. The Edit Section Assignment window is displayed.
    • Set Section to Top Layer Section.
    • Click OK.
    • Similarly assign Bottom Layer Section to the bottom layer and Core Layer Section to the core.
  8. 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 Top Layer
    • Set Instance Type to Dependent (mesh on part)
    • Click OK. The top layer is instanced in the assembly.
    • Again double-click on Instances. The Create Instance window is displayed.
    • Set Parts to Core Layer
    • Set Instance Type to Dependent (mesh on part)
    • Check Auto-offset from other instances
    • Click OK. The core layer is instanced in the assembly.
    • Click the Create Constraint: Face to Face tool. You see the message Select a planar face or datum plane of the movable instance below the viewport.
    • Click the bottom face of the top layer. You see the message Select a planar face or datum plane of the fixed instance below the vieport
    • Click the top face of the core. Arrows appear on the faces and you see the message The instance will be moved so that the arrows point in the same direction below the viewport.
    • Click OK or Flip as required to have the arrows pointing in the same direction. You see the prompt Distance from the fixed plane along its normal below the viewport.
    • Set it to 0.0
    • Similarly use face to face constraints on the other two surfaces to align the parts as displayed in the figure.
    • Again double-click on Instances. The Create Instance window is displayed.
    • Set Parts to Bottom Layer
    • Set Instance Type to Dependent (mesh on part)
    • Check Auto-offset from other instances
    • Click OK. The bottom layer is instanced in the assembly.
    • Use the Create Constraint: Face to Face tool 3 more times to align the parts as shown in the figure.
  9. Create Sets in the Assembly
    • Expand the Assembly container.
    • Double-click on Sets. The Create Set window is displayed.
    • Set Name to displacement point set 1
    • Set Type to Geometry
    • You see the message Select the geometry for the set below the viewport. Select the lower left corner of the core cell closest to the free end of the structure.
    • Click Done
    • Double-click on Sets. The Create Set window is displayed.
    • Set Name to displacement point set 2
    • Set Type to Geometry
    • You see the message Select the geometry for the set below the viewport. Select the lower left right corner of the bottom layer.
    • Click Done
  10. Create Steps
    • Double-click on Steps in the Model Database. The Create Step window is displayed.
    • Set Name to Apply Load
    • 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 the pressure load on top surface of sandwich structure.
    • Click OK.
  11. Leave Field Output Requests at defaults
  12. 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 Displacement output 1
    • Double-click on Displacement output 1 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 displacement point set 1 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 Displacement output 2
    • Set Step to Apply Load
    • Click Continue… The Edit History Output Request window is displayed
    • Set Domain to Set. A new dropdown list appears next to it.
    • Choose displacement point set 2 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
  13. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Fix Top Layer Front
    • Set Step to Apply Load
    • Set Category to Mechanical
    • Set Types for Selected Step to Symmetry/Antisymmetry/Encastre
    • Click Continue…
    • You see the message Select regions for the boundary condition displayed below the viewport
    • Select the end face of the top layer.
    • Click Done. The Edit Boundary Condition window is displayed.
    • Choose  ENCASTRE (U1=U2=U3=UR1=UR2=UR3=0).
    • Click OK.
    • Similarly create a second boundary condition called Fix Core Layer Front, applied during the Apply force step with ENCASTRE. This is applied to the end face of the core layer.
    • Create a third boundary condition called Fix Bottom Layer Front, applied during the Make Contact step with ENCASTRE. This is applied to the end face of the bottom layer.
  14. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to Uniform Applied Pressure
    • Set Step to Apply Load
    • Set Category to Mechanical
    • Set Type for Selected Step to Pressure
    • Click Continue…
    • You see the message Select surfaces for the load displayed below the viewport
    • Select the top surface of the top layer by clicking on it.
    • Click Done. The Edit Load window is displayed
    • Set Distribution to Uniform
    • Set Magnitude to 10 to apply a 10 N force in downward (negative Y) direction
    • Set Amplitude to Ramp
    • Click OK
    • You will see the forces displayed with arrows in the viewport on the surface
  15. Define surfaces
    • Expand the Assembly container in the Model Database.
    • Double-click on Surfaces. The Create Surface window is displayed
    • Set Name to Top Layer Bottom
    • Click Continue… You see the message Select the regions for the surface displayed below the viewport
    • Set it to individually with the dropdown menu
    • Select the bottom surface of the top layer. You might need to use the Replace Selected tool in the display group toolbar to display just the top layer in order to make its bottom surface visible. For the message Set entities to replace at the bottom of the viewport set the drop down item to Instances. Once you’ve selected the surface click Replace All to unhide the other part instances.
    • Similarly assign the surface Bottom Layer Top to the top surface of the bottom layer
    • Similarly assign the surface Core Layer Bottom to the bottom surface of the core
    • Similarly assign the surface Core Layer Top to the top surface of the core
  16. Assign tie constraints
    • Double click Constraints in the Model Database
    • Set Name to Tie Constraint 1
    • Set Type to Tie
    • Click Continue… You see the message Choose the master type displayed below the viewport
    • Click Surface. You see the message Select regions for the master surface individual displayed below the viewport
    • Click the Surfaces.. button at the bottom right of the viewport. The Region Selection window is displayed
    • Choose Core Layer Top. Check Highlight selections in viewport to make sure the correct surface is being selected
    • Click Continue… You see the message Choose the slave type displayed below the viewport
    • Click Surface. You see the message Select regions for the master surface individual displayed below the viewport
    • Choose Top Layer Bottom. Check Highlight selections in viewport to make sure the correct surface is being selected
    • The Edit Constraint window is displayed.
    • Leave all the settings at defaults. Click OK.
    • Repeat these steps to create another tie constraint Tie Constraint 1 with Core Layer Top as the master and Bottom Layer Top as the slave.
  17. Create the mesh
    • Expand the Parts container in the Model Database.
    • Expand Top Layer
    • 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 top layer.
    • Click Done. The Element Type window is displayed.
    • Set Element Library to Standard
    • Set Geometric Order to Linear
    • Set Family to 3D Stress
    • Check Reduced Integration
    • You will notice the message C3D8R: An 8-node linear brick, reduced integration, hourglass control
    • Click OK
    • Using the menu bar lick on Seed >Part…The Global Seeds window is displayed
    • Set Approximate global size to 0.04. Leave everything else at default values.
    • Click OK.
    • You see the message Seeding definition complete displayed below the viewport. 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
    • Repeat the same process for Bottom Layer and Core Layer.
  18. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to SandwichStructureJob
    • Set Source to Model
    • Select SandwichStructure (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Run the sandwich structure simulation
    • Set Job Type to Full Analysis.
    • Leave all other options at defaults
    • Click OK
    • Expand theJobs container in the Model Database
    • Right-click on ContactSimulationJob and choose Submit. This will run the simulation. You will see the following messages in the message window: 
      The job input file " SandwichStructureJob.inp" has been submitted for analysis. 
      Job SandwichStructureJob: Analysis Input File Processor completed successfully
      Job SandwichStructureJob: Abaqus/Standard completed successfully
      Job SandwichStructureJob completed successfully
  19. Plot mises stress and contact pressures
    • Right-click on SandwichStructureJob (Completed) in the Model Database. Choose Results.The viewport changes to the Visualization module.
    • Expand the SandwichStructure.odb container in the Results tree
    • Expand the History Output container.
    • You see two spatial displacement variables U2 for bottom layer instance and core instance.
    • Right-click on each of them and choose Save As.. Save them as SandwichXYData-1 and SandwichXYData-2.
    • 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. sandwichXYData-1 and sandwichXYData-2 should be displayed in the list. However sometimes due to a bug in Abaqus (Abaqus v 6.10 does not appear to have this bug) 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 sandwichXYData-1 to make sure it is selected.
    • Click on the Setup tab.
    • In the File section, set Name to SandwichXYData.txt in C:\SandwichFolder (you will need to create this folder).
    • 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 sandwichXYData-1 is selected.
    • Click Apply. The file SandwichXYData.txt will be written to your Abaqus working directory.
    • Click sandwichXYData-2 to make sure it is selected.
    • Click on the Setup tab.
    • In the File section, once again set Name to the same SandwichXYData.txt.
    • Check 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 sandwichXYData-2 is selected.
    • Click Apply. The file SandwichXYData.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.