Spring 2008, MET 415 - FEA Applications I

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

HW-2A, Exercise on Working Planes

Concepts:

• Basic Modeling in 2D (create shapes "By Dimensions" or by picking on the WP)
• Primitive Shapes/Boolean Operations (new operations: Overlap, Add)
• Working Plane Operations
• Meshing with "SmartSizing" vs. "Default Sizing"
  

 This cross-section of an aluminum extrusion is commonly used for residential window frames.  This part is the bottom frame for the window.  "Opening the window" is done by lifting on the extension with the round end, on the right side of the cross-section.  Of course, a pane of glass is inserted in the vertical section cut out of the main body in this shape.

• Before beginning construction: 
  • In the ANSYS Utility Menu: Workplane ->Display the Working Plane 
  • In the ANSYS Utility Menu: Workplane -> Settings 
    • use a Cartesian workplane
    • activate Grid & Triad display
    • set the WP, snap increment to 1/16"
    • use a Grid from 0 to 2" with spacing of 1/8"  
• Start by creating the large rectangular region (0.5" wide by 1.5" tall). In the ANSYS Main Menu: Preprocessing > Modeling > Create > Areas > Rectangular > Use the "By Two Corners" method and sketch it with the mouse.
• Create a rectangle on top of the first one - offset from the lower left corner by (0.1875,0.1875) inches - which is 1/8" wide and extends to the top edge of the first rectangle. **
• Add the small rectangular protrusion on the left side, 1" up from the bottom
• Add the longer rectangular protrusion on the right (0.5" wide by .125" high).
• Offset the Working Plane TO the keypoint at the far right, on the bottom edge of the right side protrusion.  In the ANSYS Utility Menu: Workplane -> Offset WP to ... -> Keypoints
• Offset the Working Plane BY Increments using -45 for the XY angle to align the WP X-axis with the inclined edge of the right side protrusion.***
• Create a rectangle which is 0.25" wide and 0.125" high in the inclined working plane coordinate system.
• Offset the Working Plane TO the keypoint at the lower end of the last rectangle (which is the center of the circular regions).
• Change the WP, snap increment to 0.05" (for the radius dimensions) - or should it be 0.025" ?
• Create a circular annulus by picking the center, inner radius, and outer radius with respect to the Working Plane Origin.
• Use the Boolean OVERLAP Operation to handle the overlapping areas ****
• Next, delete (Areas and Below) the two unnecessary area (inside the circle and inside the first large area).
• Now, handle the triangular areas: create arbitrary areas through keypoints (pick the three corners) of the two triangles which overlap the left and right sides of the original area - AND - the triangle which fills the gap in the right side protrusion.
• Use the Boolean Subtract Areas operation to subtract the two triangles from the top sides of the first large area.
• Create LINE FILLET's (radius of .05") on the (4) corners where the small rectangular features meet the thicker, vertical walls if the U-shaped section.
• Make new areas* using the fillets and the edges which were trimmed by the filleting operation.  Create Areas, Arbitrary, By Lines.
• NOW, combine all the pieces into one area, using the Boolean Operation, Add Areas.

  ---

  SUPER ! Now that you have finished that wonderful exercise in construction, its time to try meshing.

  Use a higher-order 2D plane strain finite element type and JUST MESH IT. Don't set element global size - don't set anything. See what you get with the ANSYS "Default Sizing" - annotate the no. of nodes and elements on the plot and save an image (PlotCtrls > Redirect Plots > PNG file)

  Then, in the MeshTool, find SmartSize - set it at 6, the default level and try that.
  Try lower settings for smaller element sizes and remesh.  For your final model, annotate the no. of nodes and elements on the plot and save an image 

CONSTRAIN the two vertical lines of the U-channel in the horizontal direction.
CONSTRAIN the bottom line of the U-channel in the vertical direction.
LOAD with 300 psi pressure on the bottom 90^o arc of the round feature.

Turn in:

• An element plot of the original mesh (default sizing) with the number of nodes and elements annotated on the plot.
• An element plot with the final, finer mesh density with the number of nodes and elements annotated on the plot.
• A line plot (like above) that clearly shows all the loads and constraints.
• A plot showing the deformed shape of the structure.  
  Be sure to include the mesh error measure, SEPC, in the legend of this plot.  
  (Mesh error should be < 5%)
• Plots showing the normal stresses, SX and SZ.
• A plot of the equivalent (vonMises) stress, SEQV.
• A hand calc. of the total vertical force acting on the part compared to the ANSYS total, vertical reaction force.  (Hint: projected area for the hand calc.)
  After you solve this problem, in the General Postprocessor, under List Results, Reaction Solution, get the Total FY force to compare to hand calcs.
• Also, a hand calc. of the bending, normal stress in the horizontal arm, compared to the PROPER ANSYS stress result.  Include the stress contour plot to validate your comparison.

**  If you create an AREA that is incorrect, and you want to remove it completely use: ANSYS Main Menu: Preprocessing -> Modeling -> Delete -> Areas & Below

***  If you get the Working Plane "disoriented," start over (put the WP back on the ANSYS global origin) using ANSYS Utility Menu: Workplane -> Align WP with -> Global Cartesian

****  When overlapping areas, a new area is created which is equal to the common area of the original entities. New areas are created by trimming the original areas to make room for the new area. All areas share common lines and keypoints.

* When a line fillet is created, the original lines are "broken" at the intersections with the new fillet, but a new area is NOT created.  You then form a new area using either the 3 new lines or the 3 new keypoints.  The new area is a small sliver and should be combined with the adjacent areas to avoid meshing problems.