Spring 2007, MET 415 - FEA Applications I

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

Project 2:  3D Modeling

Concepts:

• 3D Modeling:  Shell and Beam Elements
• Models with more than one Element Type & Real Constant Set (Multiple Attributes)
• Drag (Extrude) of Geometry
• Pressure Loading on Shell Elements
• Load Settings:  Gradient
• Gravity load direction
• Beam Element Usage
• Postprocessing of Shells (Top/Mid/Bott) and Mesh Error for Curved Surfaces
• Postprocessing of Beams using /ESHAPE & PowerGraphics

  A fuel oil tank for a residential oil furnace is made of sheet metal, 0.095 in. thick steel. Its dimensions are given in inches in the figure.  The leg supports are round steel pipe, 1 inch Schedule 40 steel pipe, 8 inches long. and supported in ONLY the vertical direction at the base of each leg.  The tank is completely filled with No. 2 fuel oil.

Schedule 40 pipe, 1 inch:  Cross-sect. area = 0.494 in², I = 0.08734 in⁴, O.D. = 1.315 in., I.D. = 1.049 in.  Use 3D beam elements to model the support leg (understanding that we will not have detailed stress information at the intersection of the leg and tank wall)

At the ends of the tank, where the side walls meet the end caps, the sheet metal is rolled to form the joint.  This acts as a stiffener on the tank.  Model the stiffener using 3D beam elements which have a unique set of cross-sectional properties.  Treat the rolled sheet metal as a solid square cross-section which is four times the thickness of the sheet metal in the tank walls (Cross-sect. area = 0.1444 in², I = 0.001738 in⁴, height = 0.38 in.), these elements will have the same material properties as the sheet metal.   Mesh the LINES around the perimeter of the end caps with these beams AFTER you mesh the AREAS with shell elements.

  Analyze this structure for a static loading which includes the weight of the tank and the internal pressure of the fuel oil on the tank walls (but don't actually model the oil).

Modeling Hints:

1. Check the pressure load ON THE NODE OR ELEMENT PLOTS - if the arrows point inward (when they should point outward) you need to load the "other" element face. Delete the incorrect pressures on the areas.  Then, use the LKEY to identify face 2 on those elements which need it.  In order to see the pressures on the nodes or elements before you solve, use Loads > Operate > -Transfer to FE- All Surface Loads (or All Solid Loads).

       Alternatively, you can reverse the area normal direction - see AREVERSE.

2. Define a surface load gradient BEFORE you apply the pressure to the model.

For the gradient, IF you define:

• the slope coordinate system as the global Cartesian,

• the slope direction as varying along the Y-axis, and

• the point where the slope contributes nothing to the load as the bottom of the tank

Then, the gradient is -(rho)(g/g_c)    which comes from p = (rho) * g * h  where (rho) is the density of the fluid, and

Using this gradient, you would define the highest pressure ((rho) * g * h) when you apply the pressure load. This way, at any elevation above the bottom of the tank, the pressure will decrease. It should be zero at the top of the tank.

• A table summarizing the max. stress, deflection and mesh error (SEPC) of the tank wall shell elements and the max. stress and deflection for the support leg beam elements, as well as, the end cap stiffener beam elements.

Plots showing:

• the elements (with thickness) and with real constant ID numbers identified in different colors

• the constraints and gravity load on the model

• the pressure load on the model (front and side views)

• the deformed shape (2 plots: separate the flat end of the tank from the side wall for a more correct evaluation of mesh error, 3rd plot with high stress from point load excluded)

• vonMises stress for the whole tank (top and bottom).  Consider how to present the results in spite of the point load at the top of the support leg.  Von Mises stress plot (top and bottom), separate the flat end of the tank from the side wall.

• one or two stress plots to compare with your hand calculations (mid-plane SX, SY, and/or SZ, whatever is appropriate for you calculations)

• vonMises stress plots for the support leg 

• vonMises stress plots for the stiffener beams (with /ESHAPE on).

Hand Calculation

• see, pressure vessels for an approximate stress calculation.  Compare it to the FEA results.

• verify the FEA reaction solution (S Fy = total weight of steel + oil)

• should buckling of the support leg be a design concern ?

• Include a session log file, to which you have added comments describing the process of modeling and loading the oil tank.  "Write a DB Log File" after you have constructed and successfully solved the model.  Comments are not needed on graphical picking commands (FLST, FITEM), but should be on the action command that follows the picking.  For example: 
  ASBW,P51X        !  Divide areas by WP based on graphical picking, above
  You can view a SAMPLE LOG FILE.

  ---

Reminder: All project reports will be typed, and include:

• a cover page with course name, project name, team names, and date
• a brief objective statement (2-3 sentences, maximum, of engineering objectives)
• a summary of procedures (bulleted items):
  • a complete list of assumptions, 
  • summarize the given data, 
  • highlight the modeling and analysis steps
• a conclusion statement (what was learned about the part or device, an evaluation of the design, and an interpretation of the results)
• a copy of the project statement (this web page) may be attached.