Stress Verification at Boundary Singularities

cwharpecwharpe
Recently I was modeling a square baseplate for a hydraulic column jack. Classic case of Roark's Rectangular plate with uniform central loading (the jack piston). I noted the Fixed Edges case (Table 26-8b) listed the maximum stress at the middle of the long supported edge.

How can this be verified with FEA? I read repeatedly to be skeptical of stress results at boundary locations (constraints, sharp corners, concentrated loads), and mesh refinement at those locations is often a futile chase.

Hoping there are methods known to Forum Members useful for converging a solution along boundaries(?).

Comments

  • VictorVictor
    If it really is a stress singularity, then I'd be skeptical of the meaning of the stress given in Roark's since that doesn't make sense on the face of it. Could it be that Roark's just neglects the stress due to the stress concentration in the same way that simple beam calculations ignore it it at the fixed end of a cantilever beam? The problem then becomes how to fool FEA into having the same error.

    An easy way is to use shell elements with the internal solver which neglect such bending stress concentrations.

    For solids, I wonder if you can extend the width of the plate beyond the support and move the support with it then read the stress at the original support location which is no longer a stress concentration? The displacements will be wrong but hopefully not the stresses in a linear analysis. I'm not confident that this approach is correct though since it allows deformation of the "fixed" edge.
  • cwharpecwharpe
    Yes, I think the classical solution produced by Roark neglects stress concentration at the fixed support.

    Your suggestion led me to create a rigid "picture frame" surrounding the plate, which I made rigid by increasing the Modulus by 4-6 orders of magnitude. Retained the deflection profile nicely. Smoothed, but didn't completely eliminate the hot-spots at the original edges. Had similar result by using bonded contact between picture frame interface.

    I think I'll have to employ a scheme for hot-spot averaging. Could the Stress Linearization tool into the hot-spot be useful for this? I played with it a little, but I confess whether to use or Ignore through-thickness bending stress had me confused. (What is that? -- the cylindrical/spherical radial stress?) When an SCL polled vertically across the plate thickness, "Ignoring" worked well. For a separate SCL polled across the top surface, including worked best. So, I'm a bit muddled. (I used Max Shear Stress X2 (Membrane + Bending) for reference.)

    Included file is a quadrant model of a simple 6"x6"x1/4" fixed edge plate with uniform load of 5000 lbs. Roark Theory says: At center, max def. = .0054", bend. str. = 11,088 psi. At midpt. of edge, bend stress = -24,624 psi.

    Thanks.

    ~CWimageimage
  • cwharpecwharpe
    File below.
  • rwhirleyrwhirley
    My recommendation would be to include as much of the actual support design as you can into your model. Computing power is plentiful these days, and there are many opportunities to miss important aspects of the structural response by introducing BC assumptions "too close to the action."

    The more you can make your analysis model represent the actual design, the more confidence you can have in the results.
  • VictorVictor
    edited February 2021
    I agree with rwhirley. If the goal is to verify the design, then the actual stress concentrations that it has would be important. If the goal is to verify that Roark's agrees with the idealized theory it's supposed to agree with then you might have to calculate it using that theory rather than trying to dumb down FEA results.

    That said, stress linearization sounds like a good idea. It doesn't really eliminate those high stresses, just averages them over the section (for a line through the thickness) so the peaks are lower but not as low as without the stress concentration.

    "Ignore through-thickness bending stress" excludes from the bending stress the 3 stress components that have an index in the line's direction. For the line parallel to the Z axis, it would be σ_zz, σ_yz, and σ_zx. I don't know what good this does but there's a pressure vessel code that requires it so that's why the option is there.
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register