Fall 2009, MET 425 - FEA Applications II

Prof. Dave Johnson, dhj1@psu.edu, Penn State Erie, The Behrend College

Homework Assignment: Transient Heat Transfer with Radiation

Concepts:

Heat Transfer Analysis by FEA
• Conduction
• Radiation between parts: Radiosity solver
• Transient Conditions
  • proper loading (ramped vs. stepped)
  • integration time step size
  • automatic time stepping

Problem:

A thin-walled ceramic part is placed inside a hot vacuum furnace for a short period of time to heat up.

• For the ceramic part,
  Thermal Conductivity = 120 W/(m ^oC)
  Specific Heat = 750 J/(kg ^oC)
  Density = 2850 kg/m³
  Coefficient of Thermal Expansion = 4.0x10^-6 in/in/^oC
  surface emissivity = 0.90
  

• For the brick furnace walls,
  Thermal Conductivity = 1.5 W/(m ^oC)
  Specific Heat = 1000 J/(kg ^oC)
  Density = 2000 kg/m³
  Coefficient of Thermal Expansion = 7.5x10^-6 in/in/^oC
  surface emissivity = 0.75

This model is provided to you as a ParaSolid Text File   Use a Right-click on this link, then "Save Target As...", then "Save as type: All Files", and use a file name like: "Hollow-Part-in-Furnace.x_t" 

Check the model scale after you import the geometry to ANSYS - make sure the furnace is ~0.9 m in length.

The part is initially at 22 ^oC.  The furnace walls are hot - 1600 ^oC, constant.  The environment around the furnace is 25 ^oC.  The part is to reside in the furnace for 30 seconds.

To do:

• Determine 2D or 3D modeling ?
• Determine symmetry ?
• Linear or nonlinear ?
• Will the sharp corners be a problem for thermal FEA ?
• Which radiation method to use ?
• Appropriate time step size for transient heat transfer analysis ?

Find the final temperature distribution in the ceramic part.

---

Turn in:

• Calculations for the integration time step size based on the ceramic part and its mesh.
• A geometry plot that show the different materials (materials labeled in the plot legend)
• A plot which shows ALL applied boundary conditions (environment).
• A plot which shows ALL radiating surfaces
• A final temperature contour plot of the ceramic part, alone
• A time history plot of the hottest and coldest locations on the ceramic part.
• A time history plot of the integration time step size.  INTERPRET this plot.

In ANSYS Workbench 12.0:

Create a Thermal Transient Object in the Project Schematic
Define the thermal material properties (Edit the Engineering Data)
Link the given geometry file.
Open Simulation (Edit the Model)
Assign the material properties to each body
Create "Named Selections" to (later) specify the radiation surfaces in the model
For the Transient Thermal analysis: define the initial temperature, the final time for the solution step, the initial, min, and max time step.
Define the furnace wall temperature condition (1600 C)

The only way to activate the radiosity solver for radiation is using a command object in the Thermal Analysis branch of the Tree Outline.  You first set up "Named Selections" to identify the radiation surfaces, then in the command object, you define the radiation surface conditions (SF command) and all the radiosity solver settings.  When Workbench solves the model, the radiosity solver will be used - check the "Solution Information" object to confirm.

The image above shows the "Named Selections" to identify radiation faces in the commands below:
(This is an analysis Command Object)

SF,Inside_Walls,RDSF,0.75,1
SF,Part_Faces,RDSF,0.90,1
STEF,5.67E-8     ! W/m^2 K^4
TOFFST,273       ! offset for absolute temperature
RADOPT,.1,1e-4,1,1000,.1,.1 ! Specify option for radiosity solver
SPCTEMP,1,25     ! Space TEMP (outside furnace)
HEMIOPT,10       ! Specify resolution for view factor

Add a Command Object to show/check radiation surfaces:
(This is a Solution Command Object)

/SHOW,PNG ! send plots to PNG file
/GFILE,350 ! plot file resolution
/RGB,INDEX,100,100,100,0 ! switch the
/RGB,INDEX,0,0,0,15 ! B/W colors
/PLOPT,INFO,1
/PSF,RDSF,,1
/VIEW,1,10,1,1 ! set the viewing direction
NPLOT 

Also, below "Solution" add:

• A Thermal Temperature result, scoped to the ceramic part
• A temperature probe to show the minimum temperature on the ceramic part
• A temperature probe to show the maximum temperature on the ceramic part

ANSYS Process steps:

• Set your working directory (/CWD command)
• Import the model geometry (File > Import ...)
• Use /RESET command (or PltCtrls > Reset Plot Ctrls) to reset plot controls (override wire frame)
• Main Menu: Preprocessor -> Element Type -> Add/Edit/Delete -> Add
  [Suggestion SOLID70 for furnace walls, SOLID87 for ceramic part.  WHY ?]
• Main Menu: Preprocessor -> Material Props -> Material Models >
  [Define thermal data for both materials]
• Main Menu: Preprocessor -> Meshing -> MeshTool:
  Set Global Attributes: TYPE & MAT for furnace wall
  Set a Global Element Size for furnace wall mesh
  Do a Hex, Mapped mesh of the furnace wall volumes
  Set Global Attributes: TYPE & MAT for the ceramic part
  Set a Global Element Size for the ceramic part mesh
  Do a Tet, Free mesh of the ceramic part volumes
• PlotCtrls -> Numbering -> Elem/Attrib numbering: Material numbering 
  /NUM,1 or "Numbering shown with" "Colors Only"
  
• Main Menu: Solution -> Analysis Type -> New Analysis: Transient, FULL method
• Main Menu: Solution -> Define Loads -> Apply -> Thermal -> Radiation -> On Areas
  [Pick the 4 inside walls of the furnace, define material emissivity & enclosure number]
  Picking these surfaces is tricky.  In ANSYS, click and hold the left mouse button - as you move the mouse, various entities will highlight, release the left mouse button when you have found the one you want.
• Main Menu: Solution -> Define Loads -> Apply -> Thermal -> Radiation -> On Areas
  [Pick the all surfaces of the ceramic part, define material emissivity & enclosure number]
• Main Menu: Solution -> Define Loads -> Operate-> Transfer to FE -> All Solid Lds
  [Plot elements or nodes to check definitions of radiation surfaces]
• PlotCtrls > Symbols... Under /PSF, select RDSF Emissivity, try arrows or face outlines to show proper radiation face definitions
  
• Utility Menu: Select -> Entities...
  [Select Volumes, By Num/Pick, From Full, OK.  Pick 4 volumes of furnace walls]
• Utility Menu: Select -> Everything Below -> Selected Volumes
• Main Menu: Solution -> Define Loads -> Apply -> Thermal -> Temperature -> On Nodes
  [Pick All, set a constant TEMP of 1600 on all nodes of the furnace walls]
• Utility Menu: Select -> Everything (to make the entire model active again)
• PlotCtrls > Symbols... Under /PBC, select All Applied BC's, Under /PSF, select None
  [Plot elements or nodes to check definitions of furnace wall temperature]
  
• Main Menu: Solution -> Define Loads -> Settings -> Uniform Temp
  [Define the initial TEMP of all unspecified nodes as 22]
• Main Menu: Solution -> Load Step Opts -> Time/Frequenc -> Time - Time Step
  [Enter final TIME value, initial ITS from hand calcs, choose stepped or ramped,
     Turn Auto Time Stepping ON, enter min & max ITS]
  
• Main Menu: Solution -> Load Step Opts -> Output Ctrls -> DB/Results File
  [select ALL Items for output, EVERY SUBSTEP - could make large results file]
  
• Main Menu: Solution -> Radiation Opts -> Solution Opt
  [Enter Stefan-Boltzmann constant: 5.67E-8 (SI), Offset TEMP (273), 
  Space Option: Temperature, Value: 25, Enclosure Number: 1]
• Main Menu: Solution -> Radiation Opts -> View Factor
  [if needed, change HEMIOPT setting]
• Utility Menu: File -> Save As...  [save a copy of DB before solving]
• Main Menu: Solution -> Solve -> Current LS  ->  OK
  
• Main Menu: General Postproc -> Plot Results ->Contour Plot -> Nodal Solu -> DOF Solution -> Nodal Temperature
• Utility Menu: Select -> Entities...
  [Select Elements, By Attributes, Material Number, 1 or 2, From Full, OK.  
  Pick the ceramic part to find its max/min temperatures]
• PlotCtrls -> Style -> Edge Options ... to toggle element outlines to find node numbers at MX and MN locations.  Use List -> Picked Entities > Attribute, Nodes to get the node numbers
  [Find vertex nodes ONLY.  Mid-side nodes do not have results to extract.]
  
• Main Menu: TimeHist Postpro -> to open the "Variable Viewer"
• Add data: Nodal Solution -> DOF Solution -> Nodal Temperature
  [key-in node number, HIT ENTER, then OK - do this for MN and MX nodes]
• Add data: Solution Summery -> Solution Items -> Time Step Size
• Use PlotCtrls -> Style -> Graphs ->   [to format scales, axis-labels, etc.]