March 29, 2020 at 4:05 pmstMikeSubscriber
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
March 29, 2020 at 5:33 pmpeteroznewmanSubscriber
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.
March 29, 2020 at 7:04 pmstMikeSubscriber
March 30, 2020 at 12:22 ampeteroznewmanSubscriber
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.
March 30, 2020 at 11:57 amstMikeSubscriber
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.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.