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

Modeling Contact using the Contact Pairs method in Abaqus

Last Updated:
(Published: )
This tutorial demonstrates how to simulate contact in Abaqus using the Contact-Pairs method.

New Topics Covered

  • Define surfaces in the assembly
  • Create interaction properties (specifically contact with and without friction)
  • Specify interaction pairs (contact surfaces)
  • Plot contact pressures to identify contact

Overview

In this tutorial we will analyze 3 parts that come in contact with each other using the contact pairs method (as opposed to the general contact method). The setup is displayed in the following image.

We will simulate friction between one of the contact pairs. 

The dimensions of the parts are displayed below.

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.

  1. Rename Model-1 to Contact Simulation
    • Right-click on Model-1 in Model Database
    • Choose Rename..
    • Change name to Contact Simulation
  2. Create the Plank
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Plank
    • 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 20 m and the thickness to 2 m.
    • Click Done to exit the sketcher.  The Edit Base Extrusion window is displayed.
    • Set Depth to 80.0
    • Click OK.
  3. Create the Curved Block
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Curved Block
    • 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 Circle: Center and Perimeter  tool to draw a circle
    • Use the Add Dimension tool to set the radius to 10 m.
    • Use the Create Lines: Rectangle (4 lines)  tool to draw a rectangle
    • Use the Add Dimension tool to set the height to 15 m
    • Use the Auto Trim tool to trim out parts of the circle and the rectangle to create the desired profile
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Depth to 20.0
    • Click OK.
  4. Create the Rectangular Block
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to Rectangular Block
    • 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 20 m and the height to 10 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • Set Depth to 35.0
    • Click OK.
  5. Create the 2 materials
    • 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.
    • Again double-click on Materials in the Model Database. Edit Material window is displayed
    • Set Name to Aluminum 2024-T3
    • Select General > Density. Set Mass Density to 2770 (which is 2.770 g/cc)
    • Select Mechanical > Elasticity > Elastic. Set Young’s Modulus to 73.1E9 (which is 73.1 GPa) and Poisson’s Ratio to 0.33.
  6. Assign sections
    • Double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Steel 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 Aluminum 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 Aluminum 2024 – T3 which was defined in the material creation step.
    • Click OK.
  7. Assign the sections to the parts
    • Expand the Parts container in the Model Database. Expand the part Plank.
    • 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 plank.
    • Click Done. The Edit Section Assignment window is displayed.
    • Set Section to Aluminum Section.
    • Click OK.
    • Similarly assign Steel Section to the curved block and the rectangular block.
  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 Plank
    • Set Instance Type to Dependent (mesh on part)
    • Click OK. The plank is instanced in the assembly.
    • Again double-click on Instances. The Create Instance window is displayed.
    • Set Parts to Curved block
    • Set Instance Type to Dependent (mesh on part)
    • Check Auto-offset from other instances
    • Click OK. The curved block 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 curved block. You see the message Select a planar face or datum plane of the fixed instance below the vieport
    • Click the bottom face of the plank. 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 25.0
    • 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 Rectangular block
    • Set Instance Type to Dependent (mesh on part)
    • Check Auto-offset from other instances
    • Click OK. The rectangular block 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 Steps
    • Double-click on Steps in the Model Database. The Create Step window is displayed.
    • Set Name to Make Contact
    • 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 Push parts together to avoid chatter.
    • Click OK.
    • Once again double-click on Steps in the Model Database. The Create Step window is displayed.
    • Set Name to Apply Force
    • 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 force on one end of the plank.
    • Click OK.
  10. Leave Field Output Requests at defaults
  11. Leave History Output Requests at defaults
  12. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Fix Plank End
    • Set Step to Make Contact
    • 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 shaft.
    • 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 Curved Block, applied during the Make Contact step with ENCASTRE. This is applied to the bottom of the curved block.
    • Create a third boundary condition called Fix Rectangular Block, applied during the Make Contact step with ENCASTRE. This is applied to the end face of the rectangular block.
    • Create a forth boundary condition called Press Plank Curved, applied during the Make Contact step. Set Type for Selected Step to Displacement/Rotation. Select the top surface of the plank to apply the boundary condition. When the Edit Boundary Condition window is displayed, set U2 to -1E-8 and U1=U3=UR1=UR2=UR3=0. Click OK
    • Create a fifth boundary condition called Press Rect Plank, applied during the Make Contact step. Set Type for Selected Step to Displaccement/Rotation. Select the top surface of the rectangular block to apply the boundary condition. When the Edit Boundary Condition window is displayed, set U2 to -1E-8 and U1=U3=UR1=UR2=UR3=0. Click OK
    • Right click on BCs in the Model Database. Choose Manager… The Boundary Condition Manager window is displayed
    • For the boundary conditions Press Plank Curved and Press Rect Plank, deactivate both in the Apply Force step using the Deactivate button. For the boundary condition Fix Curved Block use the Move Left button to activate it in the Initial step. For the boundary conditions Fix Plank End and Fix Rectangular Block use the Move Right button to activate them in the Apply Force step. The table should look like Table 1.
    • Click Dismiss
  13. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to Concentrated forces at corners
    • Set Step to Apply Force
    • 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 two corners of the plank by clicking on them. You will need to use the “Shift” key on the keyboard to select both of them.
    • Click Done. The Edit Load window is displayed
    • Set CF2 to -4E6to apply a 4000000 N force in downward (negative Y) direction
    • Click OK
    • You will see the forces displayed with arrows in the viewport on the selected nodes
  14. Assign surfaces
    • Expand the Assembly container in the Model Database.
    • Double-click on Surfaces. The Create Surface window is displayed
    • Set Name to rect block 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 rectangular block. You might need to suppress the face to face relationship between the rectangular block and the plank in order to make the bottom surface visible. Then resume the relationship.
    • Similarly assign the surface curved block top to the top surface of the curved block
    • Similarly assign the surface plank bottom to the bottom surface of the plank
    • Similarly assign the surface plank top to the top surface of the plank
  15. Assign interaction properties
    • Double click Interaction Properties in the Model Database
    • Set Name to Frictionless
    • Set Type to Contact
    • Click Continue… The Edit Contact Property window is displayed
    • Select Mechanical > Tangential Behavior. It is added to the Contact Property Options list.
    • Set Frictional formulation to Frictionless
    • Once again double click Interaction Properties in the Model Database
    • Set Name to Frictional
    • Set Type to Contact
    • Click Continue… The Edit Contact Property window is displayed
    • Select Mechanical > Tangential Behavior. It is added to the Contact Property Options list.
    • Set Frictional formulation to Penalty
    • Set Friction Coeff to 0.1
    • Click OK
  16. Create interactions
    • Double click Interactionsin the Model Database
    • Set Name to Curved Plank Interaction
    • Set Step to Apply Force
    • Click Continue…
    • You see the message Select the master surface displayed below the viewport
    • Set it to individually
    • Click the Surfaces… button. The Region Selection window is displayed.
    • Choose curved block top
    • Click Continue...
    • You see the prompt Select the slave type displayed below the viewport
    • Click Surface. The Region Selection window is displayed
    • Choose plank bottom
    • Click Continue...The Edit Interaction window is displayed
    • Set Contact interaction property to Frictionless. Leave all other options at default.
    • Click OK
    • Double click Interactionsin the Model Database
    • Set Name to Rectangular Plank Interaction
    • Set Step to Apply Force
    • Click Continue…
    • You see the message Select the master surface from the dialog displayed below the viewport. The Region Selection window is displayed.
    • Choose rectangular block bottom
    • Click Continue...
    • You see the prompt Select the slave type displayed below the viewport
    • Click Surface. The Region Selection window is displayed
    • Choose plank top
    • Click Continue...The Edit Interaction window is displayed
    • Set Contact interaction property to Frictional. Leave all other options at default.
    • Click OK
  17. Create the mesh
    • Expand theParts container in the Model Database.
    • Expand Plank
    • 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 plank.
    • 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 4. 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 Curved Block and Rectangular Block
  18. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to ContactSimulationJob
    • Set Source to Model
    • Select Contact Simulation (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Run the contact 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 "ContactSimulationJob.inp" has been submitted for analysis. 
      Job ContactSimulationJob: Analysis Input File Processor completed successfully
      Job ContactSimulationJob: Abaqus/Standard completed successfully
      Job ContactSimulationJobcompleted successfully
  19. Plot mises stress and contact pressures
    • Right-click on ContactSimulationJob (Completed) in the Model Database. Choose Results. The viewport changes to the Visualization module.
    • In the toolbar click the Plot Contours on Deformed Shape tool. The Mises stresses are displayed on the deformed plank and on the rectangular and curved blocks.
    • Using the Field Output toolbar change Primary to CPRESS. The contact pressures are displayed on the parts.
    • Click the Frame Selector tool and use the slider to observe contact pressures over a few frames
    • In the Display Group toolbar click the Replace Selected tool
    • You see the message Select entities to replace displayed below the viewport
    • Set it to Part instances with the dropdown
    • Click the curved block in the viewport
    • Click Done. The view of the assembly in the viewport has been replaced with the curved block.
    • Use the slider of the Frame Selector tool to go to frame 6 (last frame) of the Make Contact step. You see contact pressures displayed on the curved block indicating that contact was established in this frame.
    • In the Display Group toolbar click the Replace All tool to bring back the view of the assembly in the viewport

Table 1

Name

Initial

Make Contact

Apply Force

Fix Curved Block

Created

Propagated

Propagated

Fix Plank End

 

 

Created

Fix Rectangular Block

 

 

Created

Press Plank Curved

 

Created

Inactive

Press Rect Plank

 

Created

Inactive

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.