Fall 2007, 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

Concepts:

Heat Transfer Analysis by FEA Conduction and Convection Steady-state Conditions Convection Film Coefficients Symmetry conditions for heat transfer analyses Mesh error measure in thermal analysis (TEPC) Usage of the Element Table (ETABLE)

Thermal-Stress Analysis by FEA Coefficient of thermal expansion "Reference" Temperature reading thermal results as loads for a structural analysis

Problem:

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

• the inner layer is 1.0 inch thick concrete,
  k = 0.07 BTU/hr-in-^oF

• the outer layer is brick,
  k = 0.04 BTU/hr-in-^oF

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 2D or 3D modeling ?
• Determine symmetry ?
• Linear or nonlinear ?
• Will the sharp corners be a problem for thermal FEA ?  How about for the stress analysis ?

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.

• For the inner layer of concrete,
  E = 3,500,000 psi
  Poisson's ratio = 0.1
  Coefficient of Thermal Expansion = 5.5x10^-6 in/in/^oF
  

• For the outer layer of brick,
  E = 2,500,000 psi
  Poisson's ratio = 0.2
  Coefficient of Thermal Expansion = 3.2x10^-6 in/in/^oF 

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 70^oF
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:

• Calculations for the inside and outside convective heat transfer film coefficients (h).
• A geometry plots that show the different materials and ALL applied boundary conditions.
• A temperature contour plot. Add the mesh error in the caption for each body.
• ANSYS tabular output showing the reaction data you used to calculate the total heat flow through the ENTIRE wall of the chimney (per inch of chimney height).
• structural model constraints and applied temperature loading on an element plot
• deformed shape and contour plots of the tensile and compressive principal stresses
• Report mesh error (SEPC) for each body

For ANSYS WBE:

In 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.

In DesignSimulation: 

1. make sure the model is 2D
2. assign material properties to each part, 
3. see if "bonded contact" was created between bodies,
4. 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
5. Environment 2: thermal-stress
   1. symmetry edges
   2. insert a "Thermal Condition," Non-Uniform Temperature from the existing thermal solution
   3. A critical COMMAND OBJECT (WBE 11.0) MUST BE INSERTED UNDER "Static Structural" is:
      
      /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, "Solution Information," structural error
   5. a useful command object is:

/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