Gautam Puri
Engineer + Product Manager
This is the last article in the series titled Abaqus FEA Tutorial Series

Heat Transfer Analysis using Abaqus

Last Updated:
(Published: )
This tutorial demonstrates how to perform a heat transfer analysis with conduction, convection, and radiation using Abaqus FEA.

New Topics Covered

  • Create a steady state or transient heat transfer step
  • Assign heat flux loads and constant temperature boundary conditions
  • Use interactions to define convection and radiation heat loss mechanisms
  • Modify model attributes to define the Stefan-Boltzmann constant and absolute zero of temperature scale
  • Display nodal temperatures as a color contour using the menu and the Field Output toolbar
  • Use the Views toolbar to orient the viewport display and save custom views
  • Dock and undock toolbars in Abaqus

Overview

In this tutorial I perform a heat transfer analysis on a copper block, part of which is exposed to a heat flux, and parts of which lose heat through convection and radiation.

 

 

 

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 Heat Transfer
    • Right-click on Model-1 in Model Database
    • Choose Rename..
    • Change name to Heat Transfer
  2. Create the part
    • Double-click on Parts in Model Database. Create Part window is displayed.
    • Set Name to 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 5
    • Click OK. You will enter Sketcher mode.
  3. Sketch the profile
    • Use the Create Lines:Rectangle (4 lines) tool to draw the square profile of the block
    • Use the Add Dimension tool to set the length of the horizontal and vertical elements to 1 m.
    • Click Done to exit the sketcher. The Edit Base Extrusion window is displayed.
    • . Set Depth to 6.0
    • Click OK. The extruded block is displayed.
  4. Create the material
    • Double-click on Materials in the Model Database. Edit Material window is displayed
    • Set Name to Copper
    • Select Thermal>Conductivity. Set Conductivity to 400 (which is 400 W/mK)
    • Click OK
  5. Assign sections
    • Double-click on Sections in the Model Database. Create Section window is displayed
    • Set Name to Block Section
    • Set Category to Solid
    • Set Type to Homogeneous
    • Click Continue… The Edit Section window is displayed.
    • In the Basic tab, set Material to Copper which was defined in the create material step.
    • Click OK.
  6. Assign the section to the block
    • Expand the Parts container in the Model Database. Expand the part Block.
    • 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 block.
    • Click Done. The Edit Section Assignment window is displayed.
    • Set Section to Block Section.
    • 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 Block
    • Set Instance Type to Dependent (mesh on part)
    • Click OK.
  8. Partition the block
    • At the top of the viewport, change Module to Part using the dropdown menu.
    • Click the Create Datum Plane: Midway between 2 points tool. You see the message Select the first point to create datum plane displayed below the viewport.
    • Click on a corner (such as 0.0,0.0,0.0).You see the message Select the second point to create datum plane displayed below the viewport.
    • Click on the same corner on the opposite face (such as 0.0,0.0,6.0). You may need to use the Rotate View tool in order to be able to see that corner. The datum plane is displayed in the viewport in the middle of the block
    • Click the Partition cell: Use datum plane tool. You see the message Select a datum plane displayed below the viewport
    • Click on the datum plane to select it.
    • Click the Create Partition button below the viewport. The block is partitioned in two.
    • Click Done.
  9. Create Steps
    • Double-click on Steps in the Model Database. The Create Step window is displayed.
    • Set Name to Heating Step
    • Set Insert New Step After to Initial
    • Set Procedure Type to General >Heat transfer
    • Click Continue.. The Edit Step window is displayed
    • In the Basic tab, set Description to Apply heat in this step.
    • Set Response to Transient.
    • You may see a message Default load variation with time has been changed to Ramp linearly over step. Click Dismiss.
    • Click OK.
  10. Leave Field Outputs at default
  11. No History Outputs.
  12. Apply boundary conditions
    • Double-click on BCs in the Model Database. The Create Boundary Condition window is displayed
    • Set Name to Const Temp Surf 1
    • Set Step to Heating Step
    • Set Category to Other
    • Set Types for Selected Step to Temperature
    • Click Continue…
    • You see the message Select regions for the boundary condition displayed below the viewport
    • Select one end face of the block by clicking on it.
    • Click Done. The Edit Boundary Condition window is displayed.
    • Set Distribution to Uniform.
    • Set Magnitude to 400.
    • Click OK.
    • In the same manner create another boundary condition Const Temp Surf 2 for the opposite face of the block setting the magnitude to 350.
  13. Assign Loads
    • Double-click on Loads in the Model Database. The Create Load window is displayed
    • Set Name to Heat Flux
    • Set Step to Heating Step
    • Set Category to Thermal
    • Set Type for Selected Step to Surface heat flux
    • Click Continue…You see the message Select surfaces for the load displayed below the viewport
    • Set it to individually from the drop down list
    • Click on the top surface of the block, on the side of the partition closer to the 400 K constant temperature surface
    • Click Done. The Edit Load window is displayed
    • Set Distribution to Uniform.
    • Set Magnitude to 5000
    • Click OK
    • You will see the flux displayed with an arrows in the viewport on the selected top face
  14. Assign Interactions
    • Double-click on Interactions in the Model Database. The Create Interaction window is displayed.
    • Set Name to Convection
    • Set Step to Heating Step
    • Set Types for Selected Step to Surface film condition
    • Click Continue…
    • You see the message Select the surface displayed below the viewport
    • Select the face which will lose heat by convection by clicking on it.
    • Click Done. The Edit Interaction window is displayed
    • Set Definition to Embedded Coefficient
    • Set Film coefficient to 13
    • Set Film coefficient amplitude to Instantaneous.
    • Set Sink temperature to 200
    • Set Sink amplitude to Ramp
    • Click OK
    • Double-click on Interactions in the Model Database. The Create Interaction window is displayed.
    • Set Name to Radiation
    • Set Step to Heating Step
    • Set Types for Selected Step to Surface radiation
    • Click Continue…
    • You see the message Select the surface displayed below the viewport
    • Select the face which will lose heat by radiation by clicking on it.
    • Click Done. The Edit Interaction window is displayed
    • Set Emissivity distribution to Uniform
    • Set Emissivity to 0.78
    • Set Ambient temperature to 320
    • Set Ambient temperature amplitude to Ramp
    • Click OK
  15. Create the mesh
    • Expand theParts container in the Model Database.
    • Expand Block
    • 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 block.
    • Click Done. The Element Type window is displayed.
    • Set Element Library to Standard
    • Set Geometric Order to Linear
    • Set Family to Heat Transfer
    • You will notice the message DC3D8: An8-node linear heat transfer block
    • Click OK
    • Click Done
    • Using the menu bar lick on Seed >Part…The Global Seeds window is displayed
    • Set Approximate global size to 0.5. 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
  16. Create and submit the job
    • Double-click on Jobs in the Model Database. The Create Job window is displayed
    • Set Name to HeatTransferJob
    • Set Source to Model
    • Select Heat Transfer (it is the only option displayed)
    • Click Continue.. The Edit Job window is displayed
    • Set Description to Job simulates heat conduction through block
    • Set Job Type to Full Analysis. Leave all other options at defaults
    • Click OK
    • Expand theJobs container in the Model Database
    • Right-click on HeatTransferJob and choose Submit.
    • You will see a popup saying History output is not requested in the following steps: Heating 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 "HeatTransferJob.inp" has been submitted for analysis. 
      Job HeatTransferJob: Analysis Input File Processor completed successfully
      Job HeatTransferJob: Abaqus/Standard completed successfully
      Job HeatTransferJob completed successfully
  17. Plot heat contour
    • Right-click on HeatTransferJob (Completed) in the Model Database. Choose Results.The viewport changes to the Visualization module.
    • Using the menu bar click on Result> Field Output... The Field Output window is displayed.
    • In the Primary Variable tab, set the Output Variable to NT11 which has the description Nodal temperature at nodes.
    • Click OK
    • You see the Select Plot State window. Set Plot state to Contour. Click OK.
  18. Change view to left view
    • Expose the Views toolbar by using the menu bar and clicking on Views>Toolbars > Views.
    • Click the Apply left view button on the Views toolbar.
This is the last article in the series titled Abaqus FEA Tutorial Series
Abaqus FEA heat transfer conduction convection radiation tutorial heat flux
Did you find this article interesting?
Get notified when Gautam writes more articles:
Share Tweet Share
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.