AnsweredAssumed Answered

Frequency Study Validation

Question asked by Alec Chalmers on Jun 4, 2010
Latest reply on Jun 14, 2010 by Anthony Botting

Like • Show 0 Likes0
Comment • 7

I am having trouble validating the results of frequency studies in SW Simuation with published results and analytical calculations. In particular, I found a published result online that documents a frequency study performed in MATLAB and ANSYS with very close results that I cannot duplicate in SW Simulation. Here is the link to the document

http://www.mae.ncsu.edu/courses/mae533/klang/projects/Vibrating_Flat_Plate.pdf

SW Simulation does not even indicate the same mode shapes. Has anyone else tried to validate a frequency study?

No one else has this question

Outcomes

7 Replies

Anthony Botting Jun 4, 2010 10:44 AM
Mark Correct
Correct Answer
I get the same frequencies and mode shapes but the author of the document does not appear to specify the BC, which has a major effect on the eignevector/eigenvalue solution. I set the nodal BC on the edges of the plate for no-translation, but allow rotation, and get the same shapes and frequencies. Hope that helps. There are numerous validation sets included with the software, including NAFEMS (look in Help/SolidWorks Simulation/Validation).
Like • Show 0 Likes0
Actions
- Alec Chalmers @ Anthony Botting on Jun 4, 2010 11:01 AM
  Mark Correct
  Correct Answer
  I have been comparing results of solid models with shell models and get differing results. I assume that you used a shell model, as I haven't been able to find a restraint for solid models that allows rotation while restraining translations. In more complicated models the meshing defaults to a mix of shell and solid elements and typically we are getting lower natural frequencies with this compared with forcing all mesh to be solid.
  Like • Show 0 Likes0
  Actions
  - Anthony Botting @ Alec Chalmers on Jun 4, 2010 11:25 AM
    Mark Correct
    Correct Answer
    Yes I did use shell. You're right there's no equivalent for solids since their nodes cannot rotate, but you can make it work if you have enough computing power and time. The recommendation by FEA developers is to use at the very minium: 2 solid elements through the thickness, but ideally 3. This will help get the bending response correct (on which this model depends heavily). If your computing resources and time to mesh and solve are available, you can put a split-line in the CAD geometry right down the center (or middle) of each edge around the perimeter. This can represent a "pivot-line". When you mesh, the algorithm will attempt to put the nodes of the elements right on that line (three elements through thickness might be difficult to do that!) - use two elements through thickness and see if you get close. Now, apply a "no translation" BC on the split-line CAD geometry around the perimiter. You can probably get pretty close to the same answers as the shell model (as you probably guessed, the "shell" and "plate" type elements were specifically developed to handle these situations). Good luck on that.-Tony
    
    Message was edited by: Anthony Botting. found an image.
    Attachments
    SimulatingShellBehaviorWithSolids.png89.8 KB
    Like • Show 0 Likes0
    Actions
    - Alec Chalmers @ Anthony Botting on Jun 4, 2010 12:04 PM
      Mark Correct
      Correct Answer
      I did get the same results with shell mesh and the immovable fixture (restraint) along each edge. Using a split line on the edge of a solid mesh, how do you specify the no translation restraint; it doesn't appear to be choice for solid mesh.
      Like • Show 0 Likes0
      Actions
      - Anthony Botting @ Alec Chalmers on Jun 4, 2010 12:58 PM
        Mark Correct
        Correct Answer
        In 2010 there is a "Fixture" labeled "Fixed" (earlier versions they used the term "restraints"). Anyway, it depends what version you have, which I'm not going to research. For a "correct" method of applying "no translation", you can look for a dialog in the restraints, or fixtures, (in 2010 it's something like "Advanced Fixtures") that will allow you to choose a reference direction, say a plane. When you choose a planar reference direction, the software sets-up a local orthogonal coordinate system (this is documented in Help files). The software avails a dialog with three directions from which to choose - two in the plane at right angles, and one normal to it. You would restrain those degrees of freedom (set them to value zero).
        A shortcut is: if you use type "Fixed" and select the split-line, the software can only restrain translation X, Y and Z for solid elements, because solid element formulation includes only those degrees of freedom. If you have shell elements on that line, the term "Fixed" means restrain translation AND rotation, because shell element nodes have six degrees of freedom in their formulation (translation and rotation about each node). So, the fixture actually depends on the type of element being used.
        Like • Show 0 Likes0
        Actions
Ameer Chilakala Jun 11, 2010 3:24 AM
Mark Correct
Correct Answer
Hi,
Both solidworks simulation & ansys gives same results.

while comparing use same geometry,mesh & boundary conditions.

in that example they uses shell mesh with quadra elements then they are getting around 49 Hz.

In solidworks simulation we do not have quadra mesh, we are using triangular elements with only transulation dof fixed means we will get around 48.6 Hz.

this difference due to triangular mesh having high stifness compared to quadra elements.

Regards,
Ameer.C
Like • Show 0 Likes0
Actions
- Anthony Botting @ Ameer Chilakala on Jun 14, 2010 11:36 PM
  Mark Correct
  Correct Answer
  That is within an acceptable percentage, about 0.8%. Usually, laboratory test data cannot get that level of repeatability, so many people quit when they get simulation data within a few percent of laboratory test data - that is REALLY good. In the field, I have witnessed acceptable percentages on order of 5 to 15%.
  The triangular, 6-node, high order element can be decreased in size a bit to match the quad element stiffness (typically). Great. I'm glad you got agreement. I used to do a lot of that with ANSYS and COSMOS and have been convinced they get the "same" answer, as long as the set up is identical.
  Like • Show 0 Likes0
  Actions

Frequency Study Validation

Outcomes

Attachments

Related Content

Recommended Content