TAGGED: beam-analysis, compliance, curved-geometry
March 27, 2023 at 11:23 amAlessandro AgostinelliSubscriber
I'm trying to find the compliance factors of a curved beam flexure. The geometry is a simple curved beam (R=30mm, angle=45°) with a rectangular shape section (w=6 mm,t=1.2mm), like that:
I fixed one end and applied the force vector components (one by one) at the other one; then, I measured the displacements/rotations at the free end and divide displacement by force (or rotation by moment) to obtain the compliance factors, but I dind't get the correct results.
The correct compliance factors are analitically calculated (m/N or rad/Nm) compared to coordinate system "g" fixed at free end (like in previous picture, where x_g is red and z_g is green):
How can I do to obtain the same results with a FEA?
March 27, 2023 at 9:01 pmpeteroznewmanSubscriber
Can you calculate the correct analytic compliance factors for a straight cantilever beam? If so, please show an example.
March 27, 2023 at 9:25 pmAlessandro AgostinelliSubscriber
To calculate compliance factors for a straight cantilver beam you have to apply the components of force vector (one by one) at the free end constraining all the others DOFs. For ex., to measure compliance factor Fy - y:
The boundaries conditions are: fixed support at one end and sliding climp at other one. Solving the equation of the elastic curve of a beam, you can find the relationship between Fy and y (stiffness Fy/y, compliance y/Fy..)
March 28, 2023 at 1:18 ampeteroznewmanSubscriber
You are describing what I call a stiffness matrix. The lower left end of the shell mesh is a Fixed Support. I displace the right end with a Remote Displacement, Behavior = Rigid, keeping all other DOF = 0 except for the one unit value.
I will skip the other three load cases. In each case, I Probe the Force and Moment Reactions of the Remote Displacement.
This is a stiffness matrix. The inverse of this is the compliance matrix. This is for your geometry using Structural Steel.
Note that Finite Element Models are an approximate solution. Better approximations are obtained when the mesh is refined.
This model gives results that are closer to the expected zero values for the moments about X and Y.
March 28, 2023 at 3:03 pmAlessandro AgostinelliSubscriber
Thank you for the answer, but unfortunately I still need your help. I tried to calculate and invert the stiffness matrix for my curved beam (volume solid) in the same way you did but I didn't get the correct results.
- It's better create a CAD solid, a line body or a surface body for this type of problem? I used a CAD file, but I don't if it's correct?
2. I used shell elements..How can I choose shell mesh? It's only for Surface Bodies, it isn't..?
3. In the case you used volume solid, could be helpful the option "Beam Flexible" in Definition of the body?
4. I put Large Deflection On (because it's a "compliant part"), is it correct?
March 28, 2023 at 3:24 pmAlessandro AgostinelliSubscriber
* 2. You used shell elements..
March 28, 2023 at 4:41 pmpeteroznewmanSubscriber
- I used SpaceClaim to draw an arc, then extruded that into a sheet body with a width of 6 mm.
- That sheet body was meshed with shell elements and assigned a thickness of 1.2 mm.
- If I had used solid elements, a minimum of 4 elements through the thickness is required if using linear elements.
- Don't use Large Deflection. You want the stiffness/compliance for small displacements/rotations from the undeformed geometry.
March 28, 2023 at 5:19 pmpeteroznewmanSubscriber
The Young's Modulus I used was 2e+11 Pa. What Young's Modulus was used for the Analytic values you showed?
March 28, 2023 at 5:33 pmAlessandro AgostinelliSubscriber
The Young's Modulus is 3 GPa and Poisson's Ratio is 0,33 (is an Acrylic Plastic)
March 28, 2023 at 6:14 pmAlessandro AgostinelliSubscriber
I tried any way to obtain the correct results but I get only the compliance factors for y-Fy and thetaX-mX (where y is collinear with beam axis at free end)
I tried to improve mesh, and I used sheet, line or volume bodies but in every case I didn't solve the problem..it seems very easy but I don't get something
March 29, 2023 at 12:05 pmPeter NewmannSubscriber
Drag a new Static Structural out of the toolbox and drop it onto the Model cell of your first Static Structural analysis. Repeat this 4 times.
Open Mechanical from the A4 Model cell. Drag and drop the Fixed Support and Remote Displacement on every Static Strucural analysis, and edit each of the five Remote Displacements to move the unit displacement down the list of DOF.
What version of Ansys are you using Year and R#?
March 29, 2023 at 12:40 pmAlessandro AgostinelliSubscriber
I'm using Ansys 2023, R1
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.