Whether you can do this in Simulate depends on several factors:
- Physics associated with the system.
- How the system is designed (assembly methods, materials, etc.)
- Type of results you're after.
- Accuracy of the results.
The more information you can provide, the better. Since this is a school project, do you have a project proposal written up or part of your final report that documents the specifics of the system?
I can also run a modal analysis, but only with a low number of modes, if I try to select a range of frequency simulate runs forever.
A modal analysis determines the eigenvectors and eigenvalues of the system; i.e. the nature frequencies of the system and the mode shape associated with each. These characteristics are critical for any type of dynamic analysis (as Simulate only does linear dynamics). A key part in ensuring accurate dynamic analysis results is preventing modal truncation, which happens when you don't capture enough modes in your modal analysis and therefore truncate off the dynamic response from these missing modes. How you determine the number of modes you need depends on the type of dynamic analysis, but a good starting point is for your highest mode to be ~4x greater than the characteristics frequency of your input load. You can also run a Dynamic Frequency analysis and look at a plot of maximum displacement as a function of frequency to ensure that the response of the system at the higher modes is significantly lower than the lower modes.
I can also do the dynamic analysis and do the shock part, but don't really understand what its giving me.
There are four types of dynamic analyses in Simulate:
- Dynamic Time: This is a time-domain analysis where your loads vary as a function of time. You can simulate impulse loads (like an impact) with this, among other types of time based events.
- Dynamic Frequency: This is a frequency-domain analysis where your loads or base excitation vary as a function of frequency. A sine-sweep analysis is a good example for this.
- Dynamic Shock: This is a frequency-domain analysis where your base excitation is defined by a Response Spectrum Curve, which defines how the structure responses at a given frequency. This method is typically used to simulate seismic responses.
- Dynamic Random: This is a frequency-based analysis that uses a Power Spectrum Density as an input for loads or base excitation. This type of analysis is statistical in nature (your outputs are either PSDs or RMS values) and is usually used for inputs that are very random (think of the forcing function associated with driving over very rough terrain).
Which analysis type you use depends on the nature of your input load and the type of results you want. As I said earlier, Simulate only does linear dynamics, so all non-linear effects will be excluded. Example of non-linear effects are:
- Contact between components (i.e. path-dependent solutions).
- Material non-linearities (plasticity and hyperelasticity).
- Large-displacements and strains.
- Geometric non-linearities (e.g. loads that stay normal toa surface as it deforms).
So my question is, does simulate have the capabilities I need to be able to vary input parameters? (impact force, impact location, boundary constaints on fixture plate) In order to see what effect this will have to improve the experimental model.
Simulate does allow you to run sensitivity studies were you vary one or more parameters (e.g. geometry dimensions, load magnitude and direction, etc.) to generate a plot for certain results. However, these can be very computationally expensive to do, so it's important that you do as much work on your end with engineering judgement as opposed to just throwing it at the computer.
Im also not sure exactly what outputs simulate will give us? (an acceleration response of the fixture?)
It depends on the type of analysis, but generally speaking a dynamic analysis can give you displacement/velocity/acceleration/strain/stress/reaction forces and moments, as well as many other values as a function of your input or the total response to your input. Keep in mind that FEA is best when you know a specific result your after, as opposed to throwing a model at it and seeing what it spits out.
Our project goal is to be able to correlate the test inputs to the acceleration output and corresponding shock response spectrum.
Depending on the specifics of the systems, this should be very doable since all you're after is acceleration (as opposed to stresses).
I'll take a look at the CAD you posted. Additional information on exactly what you want to do would be very helpful.
EDIT: It looks like your Google Drive link only contains the assembly file; we'll need all the associated part files to look at your model. What you can do is create a fold in your working direction and then do a backup to that folder (File-> Save As -> Save a Backup). You can zip that folder and then upload it to Google Drive.