Define the vibrating
load sources
If your harmonic load source involves vibrating masses at various points
on the structure then 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(2pf)2
and a dynamic force of ma = mr(2pf)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(2pf)2 and a
dynamic force of ma = mr(2pf)2.
If your harmonic load source comes from base displacements, base velocities
or base accelerations then you must define them directly in the harmonic
load cases (see step 2 below) rather than as node loads. They cause
all of the base (restrained) nodes to vibrate in unison (ie. with
the same frequency, amplitude and phase). The displacements, velocities
and accelerations obtained from a harmonic analysis using a base load
source are relative to
the base (restrained) nodes.
Because vibrating loads oscillate from one side to the other there
is no need to input them as both positive and negative.
Note that if your loads are vibrating
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 harmonic
load cases
The next step involves setting
up your harmonic load cases. These can be input via the "Harmonic
Loads" datasheet. Each harmonic load case contains a source load
case (eg. a node load case that you have put your vibrating masses
into), a problem type ("Applied loads", "Base displacement",
"Base velocity" or "Base acceleration"), a mass
case (ie. the mass case that was used in the dynamic frequency analysis
on which the harmonic analysis is based), the base displacements,
velocities or accelerations (if a base load problem type was selected),
a load factor (that can be used to factor up or down the effect of
the vibrating loads), a frequency (the frequency of the vibrating
loads) and a phase (the phase of the vibrating loads).
Each harmonic load case can also contain an optional "Factor versus
frequency table" that is only used with frequency sampling to
factor up or down the effect of the vibrating loads as the frequency
changes. If no factor versus frequency table is defined then all frequencies
have the same load factor applied. If both a load factor and a factor
versus frequency table have been defined then they are multiplied
together and applied to the vibrating loads. Note that factor versus
frequency tables are not used with time sampling.
The source load case and mass case can be primary or combination load
cases.
If you want to combine vibrating loads that have different problem
types, factors, frequencies or phases into a single harmonic load
case then you can do it by simply adding extra lines with the same
harmonic load case number to the datasheet. Any lines with duplicate
harmonic load case numbers can have different source load cases, problem
types, base loads, factors, frequencies and phases. The harmonic analysis
will simply combine the effects of the duplicate lines for each harmonic
load case. Alternatively, you can combine different load sources by
the use of combination load cases.
If you want to combine harmonic analysis results with static analysis
results, refer to "Combining
harmonic and static results".
Run the harmonic
analysis
When running the
harmonic 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 sampling (time or frequency).
You can also specify the time or frequency range and the number of
time or frequency steps.
Each step is a snapshot in time (for time sampling) or frequency (for
frequency sampling) 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 harmonic analysis.
After
the harmonic analysis
After the analysis, there are four main courses of action:
(a) Animate
the structure to see how it responds to the harmonic loads.
(b) Display
graphs of displacements, velocities, accelerations and phases.
(c) Convert the time or frequency 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 harmonic loads you
can animate it via the "Show
animated dynamic response" button 
on the
side toolbar. You can choose any harmonic 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 (if time sampling is used) or versus frequency (if frequency
sampling is used) 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 harmonic
step load cases
In order to be able to use the results from a harmonic analysis in
a practical way, you can convert any of the harmonic 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 harmonic 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 harmonic step load cases with other non-harmonic load cases such
as static, spectral or transient 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 or frequency 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.
Note that step load cases cannot
be generated from a harmonic analysis that has used frequency sampling
because frequency sampling results come from a range of different
points in time and therefore do not represent an equilibrium state
of the structure.
Be careful!
If you re-run the harmonic response analysis then all the load cases
previously created from the harmonic 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 harmonic response analysis then you must carefully
check that the harmonic step load cases actually exist before you
use the results of the combination. If the harmonic 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 harmonic 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
harmonic analysis results is to look for "harmonic" in the
load case heading in analysis result reports (eg. "Load case
301 (LinComb+Harmonic)" or "Load case 302 (Harmonic)").
Generate reports
You can generate reports that
include "Harmonic Loads" (input data) and/or "Harmonic
Response" (output data). The "Harmonic 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.