Fall 2009, MET 425 - FEA Applications II

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

Homework Assignment: Steady-State Heat Transfer and Thermal Expansion/Thermal-Stress Analysis

Problem:

A very long chimney is constructed of two different materials (ignoring mortar joints): 

The chimney cross-section is shown with all dimensions in inches. All corners are sharp.
 The temperature of the hot gas inside the chimney is 140 oF.  Outside the chimney, the surrounding air is 10 oF

To do:

Determine the proper convective heat transfer film coefficients (h) for free convection of air along the vertical, flat walls, inside and outside. ASSUME (just for estimating film coefficients): the inside wall average temperature is 80 oF and the outside wall average temperature is 54 oF.  The chimney height is 28 feet.

Using the FEA solution reactions, find the total heat flow through the ENTIRE wall of the chimney (per inch of chimney height)

Find the temperature distribution through the chimney wall.

Use the same model for calculation of the thermal stress in the chimney caused only by the temperature distribution through the wall.

Since the chimney is "very long" compared to the cross-section and we choose to ignore the "end effects", plane strain behavior is the best choice.
Assume the structure is stress-free at 70oF
Apply appropriate constraints.  Apply the temperature distribution from the heat transfer solution as a (body force) load on the structural analysis model.
Evaluate deflections, tensile (S1) and compressive (S3) stress responses.

Turn in:

  1. For the Thermal Analysis:
    1. A geometry plot that show the different materials
    2. An environment showing ALL applied boundary conditions.
    3. A temperature contour plot. Add the mesh error in the caption for each body – or –  turn in the plots showing TEPC for each body
    4. (WBE) The “Details Area” info showing the reaction data from the Reaction Probe – or – (ANSYS) the total heat flow determined using the ETABLE tool
      Add a calculation of the total heat flow through the ENTIRE wall of the chimney (per inch of chimney height).
    5. (2010): Include a hand calc of heat flow through the chimney wall - treated as two concentric cylinders with inner radius 6", interface radius of 7", and outer radius of 13 in.  COMPARE the hand calc result to the heat flow value determined using the Reaction Probe.
  2. For the Static Structural Analysis:
    1. structural model constraints (environment) -OR- display the Symmetry Regions on your model 
    2. (WBE) A plot showing the “Imported Body Load” (color contours) – or – (ANSYS) applied temperature loading on an element plot
    3. deformed shape
    4. contour plot of the tensile principal stresses
    5. contour plot of the compressive principal stresses
    6. Report mesh error (SEPC) for each body – or –  turn in the plots showing SEPC for each body  
  3. Answer these questions:
    1. Should you use 2D or 3D modeling ?
    2. What  symmetry can be used in this model ?
    3. How are symmetry edges treated for heat transfer analysis ?
    4. Linear or nonlinear for heat transfer and for structural analyses ?
    5. Will the sharp corners be a problem for thermal FEA ?  How about for the stress analysis ?

For ANSYS 12.0 WBE:

In the Project Schematic, open “Custom Systems” and double-click on Thermal-Stress (to create a linked thermal and structural analysis)

Right-click in the “Steady-State Thermal”, Engineering Data cell, then Edit

In the “Outline of Schematic A2, B2: Engineering Data,” Add a new material twice, for Brick and Concrete

For each one – in the Toolbox on the left- include the properties we need for the analysis (CTE, Isotropic Elasticity, and Isotropic Thermal Conductivity).  Then, in the “Properties of Chart” for each material, enter the material data.

“Return to Project” (at the top of the screen)

Right-click in the “Steady-State Thermal”, Geometry cell, then Edit to open DesignModeler: 

  1. create 2 sketches (one for each body)
  2. make "Surface from Sketch"
  3. Use "Freeze" Tool to keep the bodies from merging
  4. "Form New Part" of the two bodies.

Make sure the model is 2D

In the Project Schematic, click on the Geometry cell for the thermal model, then click on View > Properties.  In the Properties window, set the model to 2D.  THEN, open the Model in Simulation – make sure it is 2D with the correct behavior assigned

In DesignSimulation: 

  1. assign material properties to each part, 
  2. see if "bonded contact" was created between bodies (should not be needed for a multi-body part)
  3. Environment 1: steady-state heat transfer
    1. inside convection on edges
    2. outside convection on edges
    3. how to treat symmetry in thermal analyses ?
    4. Solve for: temperature distribution, thermal error, total heat flux, insert a "Command Object" to print error TEPC, "Solution Information", use a "Reaction Probe" to find the heat transfer by convection leaving or entering the wall
  4. Environment 2: thermal-stress
    1. symmetry edges
    2. Notice: There is already an “Imported Load (Setup) > Imported Body Temperature” from the Steady-State Thermal source. 
    3. A critical COMMAND OBJECT (WBE) MUST BE INSERTED UNDER "Static Structural":

      4. /PREP7
      KEYOPT,1,3,2  ! plane strain behavior for element type 1
      KEYOPT,2,3,2  ! plane strain behavior for element type 2
      FINISH
      /SOLU
        
    4. Solve for: total deformation, maximum principal stress, minimum principal stress, insert a "Command Object" to print error SEPC, structural error
    5. a useful command object is:

      6. /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

      esel,s,mat,,1  ! select one body by material ID number
      nsle,s         ! select the nodes attached to those elements
      prerr          ! print error for that body of model
      PLDISP,1       ! plot the temperature/deflection results of that body

      esel,s,mat,,2  ! select one body by material ID number
      nsle,s         ! select the nodes attached to those elements
      prerr          ! print error for that body of model
      PLDISP,1       ! plot the temperature/deflection results of that body

      ALLSEL         ! select everything

      /SHOW,TERM     ! direct plots back to the screen