8 Replies Latest reply on Oct 7, 2014 11:30 AM by Mike Pogue

    Estimating Stress at a Known Discontinuity

    Phil Perlich

      Let me start by saying I'm in a time crunch to leave the office today. I can clean this up a bit tomorrow, but I am hoping I could get some feedback overnight.

      Capture.JPG

      Here I have a shell model for a 1/4 of a section of a cylindrical pressure vessel. It has a flat distributor plate with a design differential pressure of 40 psi. (Tank is 60" OD. The plate has 4 stiffeners)

      I need to make sure the stress in shell is not pushed too high due to the presence of the plate.

      I know I have a discontinuity at the plate to shell junction, but I still need to convince myself that the stress is not too high.

      I have plotted the stress along the edge circled in red above. (To give you an idea of the scale, the stiffener is 6" tall.) '0' is the plate-to-shell junction.

      chart.jpg

      I am utterly confused on how to interpret this data. I know you cannot interpret the design for me, but I am hoping I can get some help on how I can interpret it.

      I will post more details tomorrow if need but I hope this is enough for some help overnight.

       

      Thank you,

      Phil

        • Re: Estimating Stress at a Known Discontinuity
          Jared Conway

          you want to measure stress at the singularity

          as element size is decreasing the stress is going higher and higher

          have you already tried improving the mesh ONLY in that area and reading the stress from SEVERAL element several elements away from the singularity

          or used something like solid elements in the area to decrease the intensity of the singularity...etc

          I do not know of any way to trust or read the results in an area where there is a div 0

           

          truthfully your convergence graph should be to measure the convergence of displacement, is your solution converged?

           

          from there you will need to estimate the stress in that area based on common hand calcs, not necessarily fea

            • Re: Estimating Stress at a Known Discontinuity
              Phil Perlich

              I do want to measure the stress at the discontinuity. (Actually I do, but we all know that is not possible.)

              What I want to do is estimate the stress at the discontinuity based on the measured stresses near (but not too close to) the discontinuity.

              I thought I saw a procedure for some kind of extrapolation that I might be able to use.

               

              have you already tried improving the mesh ONLY in that area and reading the stress from SEVERAL element several elements away from the singularity

              or used something like solid elements in the area to decrease the intensity of the singularity...etc

              No, I refined the mesh globally. I will try to use a finer mesh at the discontinuity. I do not think solid elements will help me in this case.

               

              truthfully your convergence graph should be to measure the convergence of displacement, is your solution converged?

              Yes, displacement is converged, and is well within acceptable limits.

               

              from there you will need to estimate the stress in that area based on common hand calcs, not necessarily fea

              I would greatly prefer hand calcs. but I do not know of any such method for this geometry.

               

              Here is a clean version of the graph I posted yesterday.

              chart-clean.jpg

              Distance 0" is at the shell-to-plate junction (the discontinuity). Regardless of mesh size the stress values from at least 3" on are independent of mesh size.

              It appears that the near the plate (from 3" to roughly 7") the strength from the plate is reducing the stress in the shell.

              But from 0" to 3" the stress blows up. Does the discontinuity have an affect 3" away?

               

              If you stop an think about it, the plate is stopping the shell from expanding due to internal pressure. Since the shell can't expand the hoop stress would be very nearly 0. Longitudinal stress would still be present. The plate will impose a shear stress and bending stress onto the shell. Additionally, there will be a bending stress in the shell as you move away from the restraining effect of the plate.

              Perhaps I can attempt to hand calc each of these stress components and combine them.

            • Re: Estimating Stress at a Known Discontinuity
              Mike Pogue

              I'll add to what Jared wrote. Your elements are not small enough. It looks like they are about 3/4 of an inch. With shells, you could get very small elements, and you'll need to. I think the first thing you need is a failure criterion. An example would be "transverse stress at the toe of the weld = 8 ksi per ASME boiler and Pressure Vessel Code 2013" I made that up, I'm not familiar with that code. Of course, there are no singularities in real parts, so one way to estimate the stress at that corner is to linearly extrapolate from the point where it goes non linear, like in the picture below. This essentially extracts the nominal stress, which is typically what codes are based on (again, not familiar with pressure vessel codes), and ignores stress concentration. Then you can apply empirical stress concentrations, assuming they are not accounted for in the code. The trick with fatigue is, there are going to be notch stresses at the weld terminations, above and beyond geometric stress concentrations, which are probably going to drive your allowable stresses way down. You cannot model these notch stress with SolidWorks Simulation. You have to pick them up in the failure criteria/allowable stress. You also need to know how many cycles this is designed for. First cycle yielding is probably not you main problem. You also should not be comparing to the nominal strength of the material, because the weld filler and weld affected areas will not achieve a fraction of that strength--especially in fatigue. Again--look at the allowable stress and how it is defined/measured.

               

               

               

               

              linear.PNG