Community
FEA is like CFD.
Boundary Conditions make or break the simulation.
Is the real-world rail fixed for both translation and rotation at the vertical ends of the rail? Is the rider weight (Force:1) in the sim applied to the entire lower section between the bends?
Looking at the seat post for my old mountain bike, I see that the rail is only fixed for a short section of the lower section. A better model might limit the force to the clamp section of the seat post. Not all seat posts are vertical, so you may need to change the direction of the force to better match the frame geometry.
Another thought: Is there a way to fix the seat post section of the frame rail and apply forces to the ends of the rail? Have you considered how the saddle surfaces distribute the rider's weight to the rails?
What does the Free Body Diagram of the saddle/post look like? How about the Free Body Diagram of the saddle surfaces/rail? Do the reaction forces from the simulation correlate with the hand calc from the FBD? If you Right-Click on each constraint after the run, you should get the reaction forces and moments.
I've added some more FEA models to your part. Take a look at the Split feature in the model tree. It is a way to apply a boundary condition to a sub-set of a modeled surface. This may help as you translate the boundary conditions from the Free Body Diagrams to the simulation. Inventor Nastran has more options for applying loads and boundary conditions.
Mesh: Like CFD, FEA accuracy is related to mesh size. Inventor's FEA mesh sizing tools are based on the bounding box of the model. I prefer Ansys, where I can set a default element size in model units. The way around Inventor's shortcoming is to use a Local Mesh Control. Local control lets the user prescribe the mesh size in model units. The number of nodes/elements is shown in the graphics window if the user right-clicks on the mesh node and selects Mesh View.
Mesh Results:
As Posted settings: 3549 Nodes/1928 Elements, Peak Stress 496.9 MPa (1 run, default convergence setting)
1mm sizing on all model surfaces: 100504 Nodes/66021 Elements, Peak Stress 662.7 MPa (1 run, default convergence setting)
Convergence:
Take a look at the Convergence plot for each simulation. The As Posted model converged to 1.5% with the default settings. Once I changed the mesh size, I had to adjust the convergence settings to get below 10% delta between runs. There are some singularities at the model edges near the boundary conditions. They may be simulation artifacts or they may be real. Engineering judgement is required.
Note the run time for each of the sims in the model. The finer mesh and the convergence changes added time for the solutions, but not more then a minute or two on my old desktop.
Finally: Inventor's basic FEA is limited to linear loads, small displacements, and isotropic materials. Carbon fiber composites are not linear isotropic materials. If you need to understand how the layup, resin selection or other details affect the results, try Inventor Nastran, Ansys, or another FEA code that understands the physics of composite structures.
Steve Walton
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Inventor 2023
Vault Professional 2023
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
