General Mechanical

General Mechanical

How to do response of a Non_Linear(Contact) vibrating Beam

    • stMike
      Subscriber

      Good Day All


      I am currently investigating the possibility of simulating the response of a cantilever beam contact Problem undergoing Base-Excitation. The Beam will be Fixed at one end (Base) and resting on a surface with a frictionless contact relationship. As the Beam bends up it acts as a simple cantilever beam. When the beam is bending down it interacts with the surface and pivots around the edge as if around a pivot. As can be seen in the attached image I am ignoring the longitudinal displacement as the beam vibrates. I know that the Modal frequencies cannot be calculated for Non-Linear systems. Thus I would like to know if it is possible to simulate the problem to find the steady-state response of the tip of the beam when given a certain base excitation amplitude and frequency.


      I also do not know if I should model the bottom part and specify a contact relationship between the beam and the surface. Or if there is a more simplified way of specifying a frictionless surface (With possibly infinite stiffness).


      Sorry for the Hand Sketch, it is the easiest way of formulating the problem

    • peteroznewman
      Subscriber


      Use a Transient Structural analysis. Below are the instructions for a very simple model that will solve quickly.


      In SpaceClaim, Draw two co-linear lines along the X-axis, then create two Beams. The vertex between the beams is where you will attach a nonlinear spring to ground. On the Workbench Tab, click Share so the two Beams will be connected. Exit SpaceClaim.


      In Mechanical, right click on Model and insert a Connections folder. In the Connections folder, create a Translation Joint to Ground and scope it to the vertex on the left end of the beam. Edit the Joint coordinate system to point vertically.


      Now create a Spring to Ground and scope it to the vertex where you want contact. Type in the coordinates of the Reference (ground) end of the spring to give it a length and direction below the vertex. Enter a spring rate. Get the model running with a linear spring first. Later you will use a Command Object to overwrite the linear spring element with a nonlinear spring element that has a Gap capability.


      Drag the Joint to the Transient Structural to create a Joint Load. Here is where you can create a sinusoidal formula. Make sure to put at least 20 points per cycle.


      Under Analysis Settings, set the End Time for how many seconds you want. Set Large Deflection to On.  Set Auto Time Stepping to On and set the initial and minimum substeps to put 20 substeps per cycle.


      Under Damping Controls, enter the appropriate damping constants.


      Under Solution, insert a Directional Deformation result and set it for the Y axis.


      When the solution finishes, you can copy the deformation out of the result Tabular Data and paste it into Excel or Matlab where you can discard the initial transient response and keep the steady-state response.


       

    • stMike
      Subscriber

      Thank You peteroznewman for your help on this problem.


       


      Using Transient response and then waiting for it to become steady never crossed my mind. There is however one thing I would like to query. If a body-to-ground spring is used, that would imply that the spring is stationary(represented surface is stationary) while the fixed base is moving. I would like the bottom surface to be moving with the base as it would be 1 jig. How would I go about implementing this? Is it possible to add another part with same excitation frequency (taking I am using displacement function as the base excitation) and then adding some sort of body to body spring?


       


      Looking at the Hand Drawing I did I can see How confusion might occur since it looks like the base and the surface are 2 different bodies. Sorry about that


       


      Thank you for your help on this matter.

    • peteroznewman
      Subscriber

      Ah, I see. No problem.


      Create a Rigid body. Use a Fixed Joint to connect the beam to the rigid body.  Put the Translational Joint on the rigid body. Use Contact between the vertex and the face of the rigid body.



      The base is doing a 5 mm amplitude sinusoidal base displacement at about 30 Hz.


      Here is the tip response relative to the base in red (left axis) and the size of the contact gap in green (right axis).
      You can see that after 1 second, a steady state has almost developed.



      Attached is an ANSYS 2020 R1 archive.

    • stMike
      Subscriber

      Thank you peteroznewman 


      I really appreciate the help with the problem I am seeing the results I was expecting. Now it's just playing around with amplitudes and frequencies. 


       


      Thanks so much.


       

Viewing 4 reply threads
  • You must be logged in to reply to this topic.