How to Transfer Inertial Forces from Kinematic Elements for Stress Analysis
For a Mechanical Event Simulation (MES) analysis of an assembly with some parts where
the stresses throughout the analysis are not important, it is recommended to
model those parts with kinematic elements. Kinematic elements do not experience
strains and thus do not report stresses; otherwise, these elements behave just
like flexible elements. That is, they can have mass, have loads applied on their
nodes and/or faces and, most importantly, experience motion. Their advantage
over flexible elements is that they barely contribute to the size of the global
stiffness matrix. Therefore, using kinematic elements can speed up an MES
analysis.
|
If you want to determine the stresses in the kinematic element parts of the
model at a particular time step, you can then use the inertial load transfer
capability to transfer the inertial forces from the MES analysis to a copy of
the model for a static stress analysis. The inertial forces are automatically applied to the
appropriate elements in the new model in order to get the resultant stresses.
By default, the "Output data necessary for Inertial Load Transfer"
option is activated on the advanced "Analysis Parameters" screen for MES (see Figure 1). To have the inertial loads
available for subsequent transfer, make sure that this option is activated for
the MES analysis.
|
|
|
Figure 1: On the advanced "Analysis Parameters" screen for MES, make sure that the "Output data necessary for
Inertial Load Transfer" option is activated.
|
|
After the MES analysis has been run, in Superdraw, use the "File:Export:Inertial Load Transfer..."
command sequence to access the "Analysis Parameters - Inertial Load
Transfer" screen (see Figure 2). In the "Name of new model"
field, by default, your model name followed by "_ilt" will be shown as
the new filename, which will be a Superdraw drawing file (.esd) containing the
new model with the inertial forces applied.
On the "Transfer" tab, under "Groups", click on the
"Group Number" field in the "Transfer Groups" table. The
"Group Selection" pop-up window will appear, which provides a pull-down menu that will
enable you to select the group number to be transferred. Repeat this process for each group that you want
to have transferred.
By default, the "Filter MES specific element types" option is activated, which specifies that element
types that are unique to an MES analysis (actuators, sliders, contact, etc.) will not be considered
during the transfer. If you want such elements to be transferred, you must deactivate this option.
Under "Time-step", in the "Loads transferred at time-step" field, you can
specify the time-step of the MES analysis from which inertial loads will be applied.
|
|
|
Figure 2: The "Transfer" tab of the "Analysis Parameters - Inertial Load Transfer" screen.
|
|
On the "Display" tab, you can specify options for how text and
arrows from the inertial forces will be displayed in the new model (see Figure
3).
|
|
|
Figure 3: The "Display" tab of the "Analysis Parameters - Inertial Load Transfer" screen.
|
|
On the "Advanced" tab, you can specify options for "Data
transfer details", "Filters" and "Output of data" (see
Figure 4) including the following:
- Under "Data transfer details", in the "Configuration of new
model based on" field, you can use the pull-down menu to choose between
"Shape at time-step" and "Original geometry". This
option enables you to specify that the inertial forces should be applied to
either the deformed shape at the specified time-step or the original shape
of the model.
- The pull-down menu of the "Analysis type of new model" field
enables you to choose between "Linear Stress" and "MES".
- Under "Filters", if you want to specify a lower limit below which forces and
moments will not be transferred, then you can activate the "Filter transfer
loads by size" option and enter the desired limits in the "Force filter cutoff ratio"
and "Moment filter cutoff ratio" fields.
|
|
|
Figure 4: The "Advanced" tab of the "Analysis Parameters - Inertial Load Transfer" screen.
|
Press the "Perform load transfer..." button to create the new model
with the transferred inertial loads.
For more information about inertial load transfer,
see the ALGOR User's Guide.
|
