Learning Forum

[peteroznewman]

nMost structures that support machinery don't need a Static Structural model to pre-stress the structure prior to Modal analysis or a Harmonic Response.nStructures that require a Static Structural analysis to pre-stress the Modal generally have thin sections that are under high amounts of tension, for example a guitar string or the membrane of a drum head. The guitar string or drum membrane has an almost zero natural frequency when there is no tension on the structure. Once you apply the right amount of tension, you can raise that first natural frequency to the right note such as 110 Hz.nModal analysis has no loads, only mass, stiffness and supports. A machine has many parts, some of those are structural, meaning they carry load, while many other parts don't carry load such as wires, thermal or sound insulation and flimsy covers. Those parts add what is called non-structural mass (NSM). The NSM must be included in the model, but generally, those parts are deleted and only the structural parts are brought in to be meshed. ANSYS provides a way to smear that NSM over the entire structure using Distributed Mass. A few parts of the machine are concentrated massive component, such as an electric motor, or transformer. These parts are small compared with the whole structure and usually quite stiff from their own casing and bolt onto the main structure using a few bolts in a small pattern. Rather than mesh the motor casing, a Point Mass can be placed at the center of mass of the motor and a spider of elements reach back to the location of the few bolt holes that connect it to the structure. A correct Modal analysis should have the total mass equal to the actual mass of the fully assembled machine. If you don't put in all the mass, the natural frequencies will be higher than the frequencies experimentally measured on the structure.nOnce the Modal analysis has run, the resonant frequencies are known, but the amount of displacement in the Modal analysis is arbitrary because there was no load used in the analysis. To find out how much displacement will actually occur, a Harmonic Response analysis is dropped on the Solution cell of the Modal analysis. When a load is added to the Harmonic Response analysis, that is a periodic load and the magnitude is specified on the load item in the model, but the excitation frequency of that load is defined in the Analysis Settings. Typically a range of frequencies are specified and the solution tells you how much displacement magnitude every point in the model has for each excitation frequency in the analysis. The displacement is a magnitude of a periodic result that oscillates at the excitation frequency in the positive and negative directions. Obviously, the largest displacement magnitude occurs near the natural frequencies found in the Modal analysis.n