Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Airframe FEA boundary conditions

Tags:
  1. Feb 8, 2014 #1
    I'm working on a student design project building a multirotor UAV to host a sensor array. The airframe supports arm beams with motors producing thrust at the end, a battery, a flight controller, payload, ESC's and needs to be custom made so that it is of a size that can support large blades and to provide us with experience in component design.

    The only way I can see to run an FEA simulation is with a static analysis in an accelerating reference frame but I am an unsure how to define my constraints and boundary conditions (the program I am using is solidworks and it can export the model defintion to other programs such as ANSYS). Here are my current assumptions:
    1. The mounting holes to the arms are fixed realative to each other in their axial and horizontal directions.
    Justification: The frame is pocketed polycarbonate while the arm is attached with aluminium pins and supported by an aluminium tube and glass fiber reinforced blocks. Back of the envelope calculations show that the arm contact points should have deformations between 1 and 2 orders of magnitude lower than the frame.
    2. The body is in an accelerating reference frame and the other components apply forces at their mounting contact points equivalent to their mass in that accelerating frame.
    Justification: The maximum thrust dictates the maximum apparent acceleration for the entire frame.
    3. The moments can be distributed equally among all of the contact points at each arm.
    Justification: The moment of the arm is calculated from the center of thrust to the center of mass. Because the connecting bolts put the material in compression it distributes into the frame nearly as if they were made from the same material.

    Ultimately my question boils down to how do I fix the whole airframe to the reference frame? In a typical simulation the part undegoing analysis is fixed to some body that can be considered to have negligible deformation, but because this model is not tied in anyway to the earth I don't see how that should be done. I would expect each arm to bend the supporting frame structure around an axis perpendicular to the vector between the thrust center and the aircrafts center of mass with an intersection located at the center of mass. If I were to fix a single arm to the reference frame and say that the force of thrust acts on the other arms it seems that the loads I applied to the other arms would produce an additional moment around the center of the fixed point which would not otherwise be present.

    Does anyone have any other models that they would use in this situation?
     
  2. jcsd
  3. Feb 8, 2014 #2

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    If your accelerating reference frame exactly matches the thrust and weight distrubution of the UAV (for both translation and rotational accelerations) then you can fix the UAV in 6 degrees of freedom to restrain its rigid body motion, and you should get zero reaction forces to those 6 restraints.

    In priniciple it doesn't matter what 6 DOFs you choose, so long as they restrain the rigid body motions and nothing else. But to understand what went wrong if you make a mistake, it might be a good idea to fix all 6 DOFs at the center of mass of the structure.

    I don't use ANSYS, but some FE programs have an automatic procedure called "inertia relief" or something similar, to automatically calculate the correct accelerations for the acclerating reference frame based on the mass distribution of the model and the applied loads (thrust, etc). In that case, all you need to do is switch on the option, and specify the 6 DOFs to restrain the rigid body motion.

    All this depends on specifying the complete mass distribution for the structure (which might not have been required for other static analyses). It's a good idea to calculate the inertia properties of each sub-assembly of your model separately, and compare them with measured data, or at least do a sanity check that the mass and CG position look sensible. Don't forget the mass of things that might be irrelevant for the actual static analysis, like the battery, the on-board electronics, etc. You may need to model those things as "non-structural mass", e.g. additional point mass elements.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: Airframe FEA boundary conditions
  1. Boundary conditions (Replies: 18)

  2. Boundary conditions (Replies: 2)

Loading...