Spring 2006, METBD350 - FEA Applications I

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

HW 2B:  2D Modeling

Using ANSYS-Workbench:

• DesignModeler Construction
  • freeze/unfreeze tools
  • several parts to make a single body
• Scoping of Results

2D Analysis: PLANE STRAIN

A concrete dam (shown in the figure) has water pressure, its own weight, and a distributed top load.

• Modulus = 626.56 x 10⁶ lb_f/ft²
• Poisson's ratio = 0.18
• density = 143.7 lb_m/ft³
• ^{[Workbench has a set of concrete properties you may use]}

Near the center of the dam, far away from the intersection with the walls of the valley, we can treat the structure as a state of plane strain. (This is an engineering assumption)

[Sketch1, SurfaceSK1] Create a small square (~20' x ~20') at the lower right corner - for "scoping" results (after solving)

Create a small rectangle (50' x 25') [Sketch3, SurfaceSK3]  on top of the larger body (100' x 175') [Sketch2, SurfaceSK2] , aligned at the right edge.   In order to keep the bodies separate, use "frozen" for one or more.

Combine all bodies into a single part [Tools > Form New Part] before moving to simulation.  
(Don't forget to set 2D Analysis Type before entering simulation.)

You may treat the base as rigidly constrained (ALL DOF along the nodes on that edge are constrained).  

The pressure on the right side of the section shown varies linearly from 0, starting 25 ft. below the top to a maximum at the base of the dam. A linearly varying pressure loading is defined by specifying a "Hydrostatic Pressure" load on the line on the right edge of the model. For water, the weight density is 62.4 lbm/ft³, and the pressure in lb_f /sq.ft. = density * g * h.  

The weight of a structure is included in an analysis by defining the material density and by defining the gravity acceleration magnitude in the y-direction.  (Determine the proper sign/direction for the gravity load in ANSYS).  

An initial compressive load of 10000 lb_f /sq.ft. acts on the top of the dam (to simulate pre-stressed concrete).

All dimensions shown are in feet units.

Turn in:

• A plot showing the element mesh, 
• An Environment plots showing constraints, gravity vector, and the pressure loading.
• A plot showing the deformed shape (Total Deformation) of the structure.  Include the mesh error measure, SEPC, in the caption of this plot.
• Plots showing the tensile and compressive principal stresses, S1 and S3.
• A plot of the stress, SZ, perpendicular to the model's cross-section.
• A hand calculation of the mass of this structure compared to the ANSYS Total Mass (which is found in the Solution Information Window after the solution is done).
• A hand calc. of the total vertical force acting on the dam used in a comparison to the ANSYS total, vertical reaction force. 
• Also, a hand calc. of the total horizontal force acting on the dam, compared to the ANSYS total horizontal force. 
  (After you solve this problem, look under Environment at the Fixed Support object, Details area, get the Total FX and FY forces to compare to hand calcs).
• Use "scoping" to create plots of tensile and compressive principal stresses, S1 and S3, without the artificial, high levels at the overly constrained corner.