There is a structure with n degrees of freedom.The structure has forced vibration by cyclic loading. The loading period and its values depends on a parameter. in Ansys workbench how can found this parameter values cause resonance?
Hello
Your problem can be easily solved using Harmonic Response Ansys Workbench module, if your load is harmonic (sinusoidal). You just have to model your structure, apply your loading, and specify the frequency range. Peaks on amplitude graph will give you the resonance. Also you can use parametric possibilities in Ansys to automatic change in structure parameters.
Regards
the load is non-harmonic. But it can be modeled as follows:
F1+0.5*(F2-F1)*sin(w*t+pi/2)
can it be used for this load?
No, it can't. The problem is that all loads and displacements vary sinusoidally at the same known frequency (although not necessarily in phase). So, the constant force F1 is the problem.
For your case you should use Full Transient analysis. In that analysis you can use function to define your load, for example 100 + 50*sin(20*time+1.57). In this case analize the end period of time, to avoid the transient vibrations, which occur at the beginning of the excitation. So you will have manually change your parameters to obtain the results.
To reduce the calculation time you can first solve the Harmonic responce problem without constant force F1 , to define the range of possible resonance, and then perform the full transient calculations only for that range.
What obtains in this analysis? time? or the parameter that define F1 and F2 loads and w?
Could you please describe your problem in detail? Your load I understand: F1+0.5*(F2-F1)*sin(w*t+pi/2), but what parameter you want to vary? What is the goal of your analysis?
the speed of A elastic belt movment on a shaft determines the values of loads (F1,F2) and period (2pi/w). The goal is finding speeds of belt that are cause resonance on structure.
Do a static analysis for the static force component, i.e. F1. Save this results.
Do an harmonic analysis for the harmonic force component, i.e.: 0.5*(F2-F1)*sin(w*t+pi/2).
Add these results properly.
Keep in mind that the static force component will only produce a static deflection. In other words, the displacement U for dof p in the model will be the algebraic sum of the static displacement (Up_s) and the harmonic displacement (Uh_p*sin(w*t+fip)).
Up=Up_s +Up_h*sin(w*t+fip)
The harmonic analysis in ANSYS produce Up_h (the amplitude of dof p) and fip (the phase for dof p) for all w values that you specified and for all the dofs in the model.
- Badges
- Science topic