1. Limited time only! Sign up for a free 30min personal tutor trial with Chegg Tutors
    Dismiss Notice
Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Homework Help: Membrane deflection: theory vs ANSYS

  1. Jul 30, 2010 #1
    1. The problem statement, all variables and given/known data
    I am analyzing the deflection of clamped circle polysilicon membrane with radius=1500 um and thickness=1 um. The load is constant pressure ranging from 20 uPa to 20kPa.

    The problem is that my analytical solution doesn't agree with the ANSYS solution.

    2. Relevant equations
    2.1. Timoshenko gave me formulas for linear, non-linear and membrane regions of displacement. See the 1st attachment "pic1.png" for formulas and figures depicting them.

    2.2. 1st ANSYS model is axisymmetric, consists of plane42 elements
    2.3. 2nd model is made of shell181 elements
    both input files are in attachment "input.txt"

    3. The attempt at a solution
    The solution data that I get from ANSYS is on 2nd attachment "pic2.png". The ANSYS and analytical graphs differ and that's the problem. I suspect that the problem is in my ANSYS model. Any comments will be appreciated.
     

    Attached Files:

  2. jcsd
  3. Jul 30, 2010 #2

    Mapes

    User Avatar
    Science Advisor
    Homework Helper
    Gold Member

    Hi saikin, welcome to PF!

    Nice presentation. So it looks like ANSYS gives anomalously low deflection for very small pressure values, but reasonable deflection for higher pressure values? If ANSYS is set to nonlinear mode, is it possible that it's stepping up the load in increments, and there's no accurate deflection data below the smallest increment?
     
  4. Jul 31, 2010 #3
    Hi Mapes, thank you for the welcome.

    Changing the automatic time stepping to deltim,1/1000,1/2000,1/20 doesn't make any difference. Or am I getting you wrong?
     
  5. Aug 1, 2010 #4

    Mapes

    User Avatar
    Science Advisor
    Homework Helper
    Gold Member

    Not time stepping, since I assume this is a static problem. I'm talking about load stepping, in which a nonlinear, large-deformation problem is solved by applying a small load, calculating the deformation and recalculating the geometry, increasing the load, etc. I haven't used ANSYS in years, so unfortunately I can't say where these commands are. But if you're in "large-displacement" mode, it's one possibility for the anomalous low-pressure results.
     
  6. Aug 1, 2010 #5

    minger

    User Avatar
    Science Advisor

    The command I believe you're referring to is KBC and by default ANSYS will ramp the loading.

    You may want to post your mesh just so we can rule that out as a possibility for errors. Also, read carefully though the element technology guide to make sure that those plane elements are applicable.
     
  7. Aug 2, 2010 #6
    Mapes, probably I am still confused, but the ANSYS manual says:

    Substeps are points within a load step at which solutions are calculated. You use them for different reasons:
    - In a nonlinear static or steady-state analysis, use substeps to apply the loads gradually so that an accurate solution can be obtained.
    - In a linear or nonlinear transient analysis, use substeps to satisfy transient time integration rules (which usually dictate a minimum integration time step for an accurate solution).
    - In a harmonic response analysis, use substeps to obtain solutions at several frequencies within the harmonic frequency range.

    So deltim in static analysis controls the load step size.

    However, the time/load history graph looks interesting:
    1st - time-history20 kPa.png for 20 kPa load - looks the way it should be. Negative sign is ok, as it is Y axis deflection.
    2nd - time-history20 mPa.png for 20 mPa load - looks very strange. The sign changes from positive to negative at some point, which is very strange. Why there is a positive region?



    minger, please find the mesh on third pic in attachment. The plane42 seems to be suitable as it has large deflections and stress stiffening features.
     

    Attached Files:

  8. Aug 2, 2010 #7

    minger

    User Avatar
    Science Advisor

    It appears as if the second analysis doesn't use any substeps while the first one does.

    As far as the first axisymmetric analysis, exactly how are you applying the load? Can you repost the mesh with loads and constraints?
     
  9. Aug 3, 2010 #8
    minger, they both have the deltim,1/200,1/1000,1/10 specified.

    Here is the new mesh with BCs.
     

    Attached Files:

    • BCs.PNG
      BCs.PNG
      File size:
      2.4 KB
      Views:
      191
  10. Aug 3, 2010 #9
    Right now I feel kind of stupid.

    Have switched to MKS system of units (it was uMKS before that) which makes pressure range go from (20·10-12 - 20·10-3) MPa to (20·10-6 - 20·103) Pa and got an ideal agreement with theory.

    Any ideas?
    I have tried to set the small convergence value for displacements before but had no result.
     
  11. Aug 9, 2010 #10
    Unfortunately, this trick doesn't work with shell elements.
     
  12. Jul 4, 2012 #11
    Hi Saikin,

    It is an interesting verification you use, which i might want to use as well. where did you find te analytical solution for the membrane deflection? I found the linear solution in chapter 3 of timoshenko's Theory of plates and shells, but the other expresssions are harder to find.

    do you know if they are aavailable as well for square plates?

    Best Regards, Friso
     
Share this great discussion with others via Reddit, Google+, Twitter, or Facebook