Dear all,

Does anyone knows about the mathematical model for calculation of NF? The simulation result is twice of the test result. I want to use the mathematical model to investigate the difference.

Thanks

best

Dear all,

Does anyone knows about the mathematical model for calculation of NF? The simulation result is twice of the test result. I want to use the mathematical model to investigate the difference.

Thanks

best

Werther,

If you are talking about the model SolidWorks Simulation uses, it is taking the eigenvalues of the stiffness matrix. The resulting eigenvectors are the mode shapes. Incidentally, this explains why the amplitudes are arbitrary, since any multiple of an eigenvector is another eigenvector. If you are talking about a mathematical model for hand calcs, it is a pretty well understood differential equation with many common solutions and simplifications. Attached is my cheat sheet with some general stuff. If you can post at least a screen cap of your geometry and fixtures, I can help you with the specific application.

As Mike pointed out, SW is solving an eigenvalue problem, where the solution consists of the eigenvectors (mode shapes) and eigenvalues (mode frequencies) for the system. For a system with a global stiffness matrix of [K], mass matrix of [M], and global nodal displacements {d}, SW is taking:

[M]{d..} + [K]{d} = {0}

where {d..} is the second time derivative of the nodal displacements, and solving the equation:

det([M]{u}b^2 + [K]{u}) = 0

where {u} is the eigenvectors for the system, b is the eigenvalues for the system, and det() is the determinate. The eigenvector {u} is then (typically) normalized, where the maximum nodal displacement is set to 1, and all other nodal displacements are scaled relative to that.

There are a couple things to keep in mind when comparing the modal results from a numerical simulation to a physical test.

- For SW, a linear eigenvalue problem is performed. Does a linear approximation represent your system accurately enough?
- The stiffer the system is, the higher the first mode; more specifically, if you increase your system's stiffness by a factor of 4, then your first mode increases by a factor of 2. Are you accurately capturing the stiffness of your structure from a modeling perspective? Did you refine your mesh such that your results converged? Typically the system becomes "softer" as you refine the mesh (asymptotically approaching the "true" stiffness).
- The more massive the system is, the lower the first mode; more specifically, if you increase your system's mass by a factor of 4, then your first mode decreases by a factor of 2. Did you accurately capture your system's mass? Is the only mass in your system from elements themselves, or do you have remote mass points in the system? If you have remote mass points, did you make sure the "tie" them to your system is such as way as to not effect the overall stiffness? Remote mass points uses rigid links, which have an infinite stiffness associated with them. If you tie a remote mass point over a surface, then that surface becomes infinitely rigid. If you used distributed mass, then you might be missing the mass location effects.
- If your system is an assembly, what joints are used in the physical system, and what joints are used in the FEM? Are you adding stiffness to your FEM by assuming a fastened joint is equivalent to a bonded joint?
- Are the constraints in your FEM accurately representing your physical system?
- How many modes did you request SW to solve for? A "characteristic" of a modal analysis is: the more modes you solve for, the more accurate the lower modes are. The solver should be solving more modes that you request; if you request four modes, the solver should calculate 15 or so modes. However, it never hurts to set the solver for the first 5 modes, even if all you need is the first mode.

As Shaun pointed out, there are many variables when comparing physical to simulation. To start, I would recommend a problem with a known result to make sure you trust the simulation then move to your problem.

As Mike pointed out, SW is solving an eigenvalue problem, where the solution consists of the eigenvectors (mode shapes) and eigenvalues (mode frequencies) for the system. For a system with a global stiffness matrix of [K], mass matrix of [M], and global nodal displacements {d}, SW is taking:

[M]{d..} + [K]{d} = {0}

where {d..} is the second time derivative of the nodal displacements, and solving the equation:

det([M]{u}b^2 + [K]{u}) = 0

where {u} is the eigenvectors for the system, b is the eigenvalues for the system, and det() is the determinate. The eigenvector {u} is then (typically) normalized, where the maximum nodal displacement is set to 1, and all other nodal displacements are scaled relative to that.

There are a couple things to keep in mind when comparing the modal results from a numerical simulation to a physical test.