General Mechanical

General Mechanical

Why is the deflection for my analytical solution not matching ANSYS results

    • edasinor
      Subscriber

      Hello!

      I'm currently modeling a fixed support circular plate under uniformly distributed load with a 0.381mm thickness. For a pressure of 0.005 psi, the maximum deflection is 0.1143 for my ANSYS results. However, when calculating analytically, the maximum deflection is 0.0625mm using this formula (w = pa^4/64D where D = Et^3/(12(1-v^2)) ). I used the same elastic constants. Can someone please help me.

    • peteroznewman
      Subscriber
      nWhat is you goal? Is it to make a model that gives the same answer as an equation?nOr is it to make a model that will best predict reality? Because those are two different models.nFor example, people calculate beam deflection using Euler-Bernoulli beam equations. ANSYS beam models don't give the same answer as those equations because the ANSYS BEAM188 elements use the Timoshenko beam theory and include shear which the Euler-Bernoulli beam equation does not.nAnother example is equations that use a small displacement assumption. ANSYS models that have turned on Large Deflection are performing a nonlinear solution so will give a different answer than the equation based on the small displacement assumption.n
    • edasinor
      Subscriber
      Thank you, Peteroznewman!nMy goal is to get the same answer as the ANSYS simulation. The pressures are very small so both linear and nonlinear solution gives the same answer for maximum deflection. I actually tried turning on Large deformation and turning it off and they both give the same answer because the deflection is less than the thickness of the plate. My analytical calculation does not much the ANSYS solution. nIs ANSYS using a different equation or model when calculating circular plate than w = pa^4/64D?nThank you.n
    • peteroznewman
      Subscriber
      nThere are several online calculators such as this one:nhttps://www.efunda.com/formulae/solid_mechanics/plates/calculators/cpC_PUniform.cfmnI would type in your inputs to check your calculation, but you didn't provide all the inputs.nI can't tell if you have meshed a surface with shell elements, which is the right way to do this model.nOr if you have meshed a solid body with solid elements, which is the wrong way to do this model.nANSYS is not using the formula, it is using the Finite Element Method to obtain a numerical result for the given boundary conditions.nThe advantage of the FEM is a result can be obtained for any shape, whereas the equation is only valid for a circular plate with a clamped edge.n
    • edasinor
      Subscriber
      Hi Peteroznewman,nYes, I used the online calculator at a point. My input parameters; diameter of the plate = 50mm, hence a=25mm; young modulus (E) = 575 mpa; poission ratio (v) =0.46; pressure (P) = 0.005psi; thickness of the plate is 0.381mm.nThe plate is a surface body modeled in Design Modeller. However, I'm not sure which shell element was selected during meshing. Did I make any mistake with the setup?nThank you.n
    • peteroznewman
      Subscriber
      nYou have made a mistake somewhere. Below is my model result and the calculator result. They agree within 4%.n
    • edasinor
      Subscriber
      Hello Peteroznewman,nThank you so much for your help!nIs it because I used symmetric geometry? I tried troubleshooting but I couldn't find where I made a mistake. n
    • peteroznewman
      Subscriber
      nTry a full model.n
    • peteroznewman
      Subscriber
      Correction to my earlier post, the ANSYS result agrees within 0.4% of the analytical equation.n
    • edasinor
      Subscriber
      Thank you, Peteroznewman.nnThe full model worked. Apparently, I didn't add symmetry boundary conditions. Thanks for your help.n
Viewing 9 reply threads
  • You must be logged in to reply to this topic.