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

edasinor
Member Posts:

**5**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.

Tagged:

## Answers

11,369@edasinor

What is you goal? Is it to make a model that gives the same answer as an equation?

Or is it to make a model that will best predict reality? Because those are two different models.

For 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.

Another 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.

5Thank you, Peteroznewman!

My 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.

Is ANSYS using a different equation or model when calculating circular plate than w = pa^4/64D?

Thank you.

11,369@edasinor

There are several online calculators such as this one:

https://www.efunda.com/formulae/solid_mechanics/plates/calculators/cpC_PUniform.cfm

I would type in your inputs to check your calculation, but you didn't provide all the inputs.

I can't tell if you have meshed a surface with shell elements, which is the right way to do this model.

Or if you have meshed a solid body with solid elements, which is the wrong way to do this model.

ANSYS is not using the formula, it is using the Finite Element Method to obtain a numerical result for the given boundary conditions.

The 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.

5Hi Peteroznewman,

Yes, 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.

The 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?

Thank you.

11,369@edasinor

You have made a mistake somewhere. Below is my model result and the calculator result. They agree within 4%.

5Hello Peteroznewman,

Thank you so much for your help!

Is it because I used symmetric geometry? I tried troubleshooting but I couldn't find where I made a mistake.

11,369@edasinor

Try a full model.

11,369Correction to my earlier post, the ANSYS result agrees within 0.4% of the analytical equation.

5Thank you, Peteroznewman.

The full model worked. Apparently, I didn't add symmetry boundary conditions. Thanks for your help.