MET 415 - FEA Applications I

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

HW 2B:  2D Modeling

2D Analysis: PLANE STRAINdam2.gif (5169 bytes)

A concrete dam has water pressure, its own weight, and a distributed top load.  All dimensions shown are in feet units.

Element Type > Add/Edit/Delete > pick an appropriate 2D element.  Then, SET the Element OPTIONS !!!

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)

Create a small rectangle (50 x 25) on top of a larger rectangle (100 x 175), aligned at the right edge.  Use the WP to divide the upper left corner of the larger area.  Delete that corner, then GLUE (or ADD) the remaining areas.

You may treat the base as rigidly constrained (ALL DOF along the nodes on that edge are constrained).  >Loads >Define Loads >Apply >Structural >Displacement >On Lines

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 different pressure value at the top and bottom of a line on the right edge of the model. For water, the weight density is 1.94 slugs/ft3, and the pressure in lbf /sq.ft. = density * g * h.  >Loads >Define Loads > Apply >Structural >Pressure > On Lines...  with a different value at each end of the line.

[The pressure load will vary from one end to the other, but which end is which ?  One approach: guess and check when the load is transferred to the mesh.  If it's wrong, redefine, switch the load values at the start end (I) and the other end (J)]

The weight of a structure is included in an analysis by defining the material density (DENS) and by defining the gravity acceleration magnitude (32.2 ft/sec2) in the y-direction.  (Research the proper sign for the gravity load in ANSYS).  >Loads >Define Loads > Apply >Structural >Inertia >Gravity >Global

An initial compressive load of 10000 lbf /sq.ft. acts on the top of the dam (to simulate pre-stressed concrete). >Loads >Define Loads > Apply >Structural >Pressure > On Lines... with a constant value on the top edge

[Make sure you do NOT use a varying pressure load on the top edge]

USE Solution >Loads >Define Loads >Operate >Transfer to FE >All Solid Loads to see all loads and constraints on the nodes and elements

Turn in:

  1. A plot showing the elements, constraints, gravity vector, and the pressure loading.
  2. A plot showing the deformed shape of the structure.  Include the mesh error measure, SEPC, in the legend of this plot.
  3. Plots showing the tensile and compressive principal stresses, S1 and S3.
  4. A plot of the stress, SZ, perpendicular to the model's cross-section.
  5. Calculations:
    1. A hand calculation of the mass of this structure compared to the ANSYS Total Mass (which is found in the Output Window after the solution is done).
    2. A hand calc. of the total vertical force acting on the dam used in a comparison to the ANSYS total, vertical reaction force. 
    3. 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, in the General Postprocessor, under List Results, Reaction Solution, get the Total FX and FY forces to compare to hand calcs).
  6. Answer this question: Why do we need to > Operate >Transfer to FE > All Solid Loads in order to view the boundary condition BEFORE we solve the model ?  [We know that ANSYS automatically transfers ALL loads and constraints from the solid model to the nodes and elements when we solve]