Piezoelectric Cantilever Beam Boundary Condition

Ammar676Ammar676 Member Posts: 5
edited April 5 in Structures

Hello everyone,

I am trying to simulate a piezoelectric cantilever beam. I am facing a small issue in the boundary conditions. how can I apply AC magnetic field in the beam. Note that the cantilever beam is made of brass sheet sandwiched between to PZT-5H bodies and there are two neodymium magnet at the end. The magnets are supposed apply a magnetic force moment from the AC magnetic field generated by helmholtz coils. But I don't know how to apply ac magnetic field into the beam.

I only have access to the student free version of ANSYS. Please tell me if I can do it on the free version or not.

Thanks

Answers

  • wrbulatwrbulat Posts: 28Forum Coordinator

    What a FUN project!

    1) Sorry, I don't know for sure whether or not the license associated with your academic version will allow you access to the technology, but I think it will. The documentation shows that the SOLID226 coupled field element (used for both piezoelectric and coupled magnetostructural analyses) has no "product specific restrictions":


    2) What release are you using, and are you using (a) the Piezo and MEMS ACT with an older version of Mechanical, (b) the fairly recently introduced coupled field system that is natively exposed in Workbench, or (c) the MAPDL solver directly? That's right, there are a multiplicity of ways of accessing the technology and setting up the model for the an analysis like this. Oh, there's yet another possibility - system coupling between Maxwell and Mechanical. The only application in which the magnetostructural and electromagnetostructural options of SOLID22x are exposed is option (c). So options (a) and (b) would require command objects to modify element keyoptions in domains to convert element types, and also to apply boundary conditions. Please try to locate the Help on SOLID226/227 to review the options these element types offer. If you have modest to good understanding of/proficiency in APDL, option (c) may be the least problematic/most straightforward. Being old and grouchy, I would choose (c) if I were tasked with this analysis.

    3) Considerations: what is the frequency of the oscillating B field? Both the beam and the **** are electrically conductive. In the presence of a time-varying B field, eddy currents will be induced in these bodies, shielding their interior from the field and altering the field in the free space adjacent to them. There will be volumetrically distributed Lorentz forces associated with these eddy currents which may (or may not) be comparable to the magnetic forces acting on the ****. The velocity effect might contribute still further to the production of eddy currents. EMF and associated electrical currents are induced in moving conductors as they pass through magnetic fields. The magnitude of these effects is frequency dependent. In slowly varying fields they are almost surely negligible. If they need to be accounted for, then use KEYOPT(1)=10101 for the beam and ****. They will then have the AZ, VOLT, and UX/Y/Z DOFs (electrically conductive structures through which magnetic fields pass)

    4) There's an APDL command for defining a uniform external B field:


    My first thought is to create a do loop (*DO and *ENDDO commands). In each pass through the loop, advance time (TIME command), use the DFLX command with a different value of magnetic flux density (you can use an expression in the fields of the command to define it such that it varies harmonically in time), and solve.

    5) For the piezo bodies, you might need two sets of elements that use the same mesh nodes. One set of elements would be piezoelectric - these would produce a voltage signal in response to mechanical deformation. The other set would be magnetostructural to calculate the propagation of the magnetic field through the piezoelectric bodies. You can use the EGEN command with a zero node number offset to create the duplicate set of elements from an existing set. MAPDL allows this - I've done it many times.

    6) All of the bodies comprising the system should be defined as a single part so that mesh nodes on all interfaces are shared by the elements on either side. There is no magnetic contact element compatible with edge-flux magnetic formulation, so the mesh must be conformal.

    I hope this gives you a place to start. I've never done exactly this myself, but from my experience with both piezoelectric and magnetostructural analyses my confidence is high that it's possible.

    Kind regards,

    Bill

  • Ammar676Ammar676 Posts: 10Member

    Thank you so much Bill for your time.

    But to be honest, I have never used APDL commands before.

    Do you think is there any other way to do it?


    Kind regards,

    Ammar

  • Ammar676Ammar676 Posts: 10Member

    Forgot to mention that I using ANSYS Workbench not ANSYS APDL.

    I should've been more clear about this. My bad!

Sign In or Register to comment.