The steps required to prepare the input data for a transient analysis, run the analysis and then obtain results are described below.

Define the time-dependent load sources

You need to define your time-dependent load sources in different ways depending on their type as follows:

"Applied loads" are general purpose time-dependent loads that you must apply to the structure as normal static node loads. The time-dependent properties of the loads are defined separately when you create your transient load cases as described below.

"Initial displacements" are assumed to be present at time zero and are immediately removed, causing the structure to react and settle into a new state of equilibrium. They typically come from the analysis results of a static or spectral load case. You simply need to specify the load case that they come from as the "Source case" when you create your transient load cases as described below.

"Initial velocities" are assumed to be present at time zero and are immediately removed, causing a structural response. Because there is currently no dedicated datasheet for velocities, you must input the initial velocities as node loads but with units of length/sec and radians/sec instead of forces and moments, where "length" is the length unit used in the job.*Note that if you change the job length, force or moment units, the "velocity" node loads may no longer be correct and it is up to you to convert them manually*.

"Base acceleration" applies time-dependent in-phase translational or rotational accelerations to the base (restrained) nodes. They cause all of the base nodes to vibrate in unison. You simply define them in the transient loads datasheet when you create your transient load cases as described below. For rotational accelerations you must also specify the node that the rotations act about. The displacements, velocities and accelerations obtained from a transient response analysis using a base acceleration load source are__relative to the base (restrained) nodes__, and so if you want to obtain the net displacements, velocities or accelerations then you need to superimpose the base displacements, velocities or accelerations on the reported values, taking into account that they could be in opposite directions.

"Harmonic loads" involve masses vibrating in a sinusoidal motion at various points on the structure. The first step requires you to calculate their dynamic force and input them as node loads. The dynamic force of a vibrating mass is its mass multiplied by its maximum acceleration. For example, a mass*m*rotating about a circle of radius*r*with a frequency of*f*has a maximum acceleration of*a = r(2**p**f)**2*and a dynamic force of*ma = mr(2**p**f)**2*. This is also equal to the centrifugal force of the rotating mass. Similarly, a mass*m*moving linearly in harmonic motion (eg. like a piston) over a travel distance of*2r*with a frequency of*f*also has a maximum acceleration of*a = r(2**p**f)**2*and a dynamic force of*ma = mr(2**p**f)**2*. Because harmonic loads oscillate from one side to the other there is no need to input them as both positive and negative.

"Periodic loads" are similar to harmonic loads except that they follow an arbitrary time-dependent repeating pattern rather than being strictly sinusoidal. You should apply them as normal static node loads. Their period and time-dependent properties are defined separately when you create your transient load cases as described below.

*Note that for all load types, if they are acting at some angle to the global axes then you must calculate their global components and apply them in each of the global directions*.

Create the transient load cases

The next step involves setting up your transient load cases. These can be input via the "Transient Loads" datasheet. Each transient load case contains a source load case (eg. a node load case that you have put your time-dependent loads or velocities into or an analysed load case that contains initial displacements), a problem type ("Applied loads", "Initial displacements", "Initial velocities", "Base acceleration", "Harmonic loads" or "Periodic loads"), a mass case (ie. the mass case that was used in the dynamic frequency analysis on which the transient analysis is based), the base accelerations (if the "Base acceleration" problem type was selected), a load factor (that can be used to factor up or down the effect of the time-dependent loads), a frequency (for harmonic loads), a phase (for harmonic or periodic loads) and a period (for periodic loads).

Each transient load case also contains a "Factor versus time table" that defines the time-dependent properties of the applied load, base acceleration and periodic load sources. If no table is defined then the load source is just assumed to be suddenly applied at time zero and held constant. Harmonic loads generally don't require a factor versus time table, however a table can be defined to further vary the time-dependent effect of a harmonic load source if required. If both a load factor and a factor versus time table have been defined then they are multiplied together and their product is applied to the transient loads.

The source load case and mass case can be primary or combination load cases.

If you want to combine load sources that have different problem types, factors, frequencies, periods, phases or time-dependent properties into a single transient load case then you can do it by simply adding extra lines to the datasheet that have the same transient load case number. Any lines with duplicate transient load case numbers can have different source load cases, problem types, base acceleration, factors, frequencies, periods, phases and factor versus time tables. The transient analysis will simply combine the effects of the duplicate lines for each transient load case.

If you want to combine transient analysis results with static analysis results, refer to "Combining transient and static results".

Run the transient analysis

When running the transient analysis you can select which dynamic modes to consider (usually just leave the mode list blank to consider them all), the damping type (none, modal or Rayleigh) and the number of time steps.

Each step is a snapshot in time at which the structural response is calculated. You should choose the number of steps based on a good compromise between analysis speed, the amount of data that gets generated, and enough sampling points to get a good representation of the structure's response. 1000 steps is usually a good starting point. If you set it too low then you may miss some of the peaks and troughs in the structure's response if they happen to occur between steps. If you set it too high then the analysis will be slower and the amount of data stored with the job will be larger. The number of steps also has a direct affect on the smoothness of the animation and graphs that you can get after the transient analysis.

After the transient analysis

After the analysis, there are four main courses of action:

(a) Animate the structure to see how it responds to the transient loads.

(b) Display graphs of displacements, velocities, accelerations and phases.

(c) Convert the time steps to step load cases.

(d) Generate reports of the results.

These are explained in more detail as follows.

Animate the structure

In order to see how the structure responds to the transient loads you can animate it via the "Show animated dynamic response" button on the side toolbar. You can choose any transient load case to animate and specify the animation speed. An animation speed of "1x" shows it in real-time.

Display graphs

Graphs of displacements, velocities, accelerations or phases versus time can be displayed by right-clicking on any node and then selecting "Harmonic/Transient Response Graph" from the popup menu that appears. Once the graph has appeared, you can change load cases via the load case selector at the top of the graph and you can change the diagram type or axis via the "Diagram Type" button.

You can also click on any other nodes while the graph is visible and it will be updated for each node that you click.

Generate transient step load cases

In order to be able to use the results from a transient analysis in a practical way, you can convert any of the transient time steps to load cases that contain displacements, forces, moments, stresses and reactions, just like you would get from a static analysis. You can do this by selecting "Generate Dynamic Response Step Load Cases" from the "Loads" menu, choose the transient load case that you want to create the load cases from and then specify the starting load case number. You can also use this tool to generate combination load cases that combine the transient result load cases with other non-transient load cases such as static, spectral or harmonic load cases.

You must first decide which steps you want to convert to load cases. It is usually a good idea to only convert the steps that correspond to peaks or troughs in the structure's response, otherwise you may generate many load cases that are of no use. You can specify a list of steps to be converted or you can request SPACE GASS to search for the peaks and troughs by selecting "Steps at min/max values". You can also limit the steps to a specific time range.

Multiple options can also be selected. For example, if you specify a step list of 500-700, tick "Steps at min/max values" and specify a time range of 4-6 seconds then SPACE GASS will choose the steps between 500 and 700 that correspond to peaks and troughs within the time range of 4 to 6 seconds. If you make your search too restrictive then you may exclude all steps. Conversely, if you convert too many steps to load cases then you may finish up with a huge number of unwanted load cases.

Once the step load cases and combinations have been generated then you can view them, get reports and use them in any of the design modules, just like any other load cases.

*Be careful! If you re-run the transient response analysis then all the load cases previously created from the transient steps will be deleted and you will have to re-generate them!*

.*If you have a combination load case that combines static load cases with step load cases from a transient response analysis then you must carefully check that the transient step load cases actually exist before you use the results of the combination. If the transient step load cases have been deleted (due to a model, load or mass change or a re-analysis) then the combination may just contain the results of the static load cases. Because SPACE GASS allows combination load cases to include non-existent load cases, it doesn't give any warnings or errors if the transient step load cases are missing. It can't even detect that they are missing because they have no input data associated with them. One way for you to quickly check if combination load cases contain transient analysis results is to look for "transient" in the load case heading in analysis result reports (eg. "Load case 301 (LinComb+Transient)" or "Load case 302 (Transient)")*

Generate reports

You can generate reports that include "Transient Loads" (input data) and/or "Transient Response" (output data). The "Transient Response" report includes a list of the nodes and steps that correspond to the locations of maximum translation, velocity, acceleration and rotation. These are sometimes useful for finding the critical locations in your model.