The mode-superposition method scales the mode shapes obtained from a modal analysis and sums them to calculate the dynamic response. For more detailed information, see Mode-Superposition Method in the Mechanical APDL Theory Reference.
The procedure to use the method consists of five main steps:
Build the model.
Obtain the modal solution.
Obtain the mode-superposition transient solution.
Expand the mode-superposition solution.
Review the results.
Building the model for a mode-superposition transient dynamic analysis is the same as that described for the full method. See Build the Model for more information.
Modal Analysis describes how to obtain a modal solution. Following are some additional hints:
The mode-extraction method should be Block Lanczos, PCG Lanczos, Supernode, Subspace, or QR damped. (The other methods, Unsymmetric and Damped, do not apply to mode-superposition.) If your model has damping and/or an unsymmetric stiffness matrix, use the QR Damp mode-extraction method (MODOPT,QRDAMP).
Be sure to extract all modes that may contribute to the dynamic response.
If you use the QR damped mode-extraction method, specify damping as follows:
Specify global damping in the modal or mode-superposition analysis (ALPHAD, BETAD, DMPSTR).
Specify material (MP,ALPD, MP,BETD, MP,DMPS, TB,SDAMP,,,,ALPD, TB,SDAMP,,,,BETD) and element dependent damping (COMBIN14, MATRIX27, MATRIX50) in the modal analysis.
Specify damping ratios in the mode-superposition analysis (DMPRAT, MDAMP).
For more details about damping definition, see Damping.
Specify displacement constraints, if any. Note that additional constraints may not be applied in the subsequent mode-superposition transient analysis.
If you need to apply element loads (pressures, temperatures, accelerations, etc.) in a transient dynamic analysis, you must specify them in the modal analysis. The loads are ignored for the modal solution, but a load vector will be calculated and written to the mode shape file (Jobname.mode), and the element load information will be written to Jobname.mlv. You can generate multiple load vectors (see the MODCONT command in Generating and Using Multiple Loads in Mode-Superposition Analyses). You can then scale and use these load vectors in the transient solution.
To include the contribution of higher frequency modes in the subsequent transient analysis, you can calculate the residual vectors or residual responses in the modal analysis (see the RESVEC command in Using the Residual Vector or the Residual Response Method to Improve Accuracy).
If the transient excitation is coming from the support, you can generate pseudo-static modes needed in the subsequent transient analysis (see the MODCONT command in Enforced Motion Method for Mode-Superposition Transient and Harmonic Analyses).
You should expand the modes and calculate the element results to save computation time in the subsequent expansion of the transient results (MXPAND,ALL,,,YES,,YES). Do not use this option if you are applying thermal loads (see Option: Number of Modes to Expand (MXPAND) in this guide for details about this limitation). The model data (for example, nodal rotations) should not be changed between the modal and transient analyses.
You can select the modes of interest for the expansion. Because the expansion is performed on selected modes only, you will save computational time in the subsequent mode-superposition transient analysis. See Using Mode Selection for information about this procedure.
If groups of repeated frequencies are present, make sure you extract all the solutions in each group. For more information, see Repeated Eigenvalues in the Mechanical APDL Theory Reference.
In this step, the program uses mode shapes extracted by the modal solution to calculate the transient response. The following requirements apply:
The mode shape file (Jobname.mode) must be available.
The full file (Jobname.full) must be available if linear acceleration (ACEL) is present in the mode-superposition analysis, or if coupling and/or constraint equations are present in the model, including constraint equations created during the solution by certain element types (contact elements, MPC184, and so on).
The database must contain the same model for which the modal solution was obtained.
The element modal load file (Jobname.mlv) must be available if load vectors were created (MODCONT,ON) and the element results were written on the Jobname.mode file (MSUPkey = YES on the MXPAND command) during the modal analysis.
The procedure to obtain the mode-superposition transient solution is described below:
Enter SOLUTION.
Define the analysis type and analysis options. These are the same as the analysis options described for the full method (in Set Solution Controls and Set Additional Solution Options), except for the following differences:
You cannot use the Solution Controls dialog box to define analysis type and analysis options for a mode-superposition transient analysis. Instead, you must set them using the standard set of solution commands (which are listed in Set Solution Controls and Set Additional Solution Options) and the standard corresponding menu paths.
Restarts are available (ANTYPE).
Select the mode-superposition method of solution (TRNOPT).
When you specify a mode-superposition transient analysis, a menu appropriate for the specified analysis type appears. The menu will be either "abridged" or "unabridged," depending on the actions you took prior to this step in your session. The abridged menu contains only those solution options that are valid and/or recommended for mode-superposition transient analyses. If you are on the abridged menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the option from the menu. For details, see Using Abridged Solution Menus in the Basic Analysis Guide.
Specify the number of modes you want to use for the solution (TRNOPT). This determines the accuracy of the transient solution. At a minimum, you should use all modes that you think will contribute to the dynamic response. If you expect higher frequencies to be excited, for example, the number of modes specified should include the higher modes. The default is to use all modes calculated in the modal solution.
To include the contribution of higher frequency modes, add the residual vectors calculated in the modal analysis (RESVEC,ON).
If you do not want to use rigid body (0 frequency) modes, use
MINMODEon the TRNOPT command to skip over them.By default, reaction force and other force output contains only static contributions. If you want to postprocess the velocities, accelerations, and derived results (
Lab= TOTAL, DAMP or INERT on FORCE), useVAouton TRNOPT.
Apply loads to the model. The following loading restrictions apply in a mode-superposition transient dynamic analysis:
Only nodal forces (F, FK) and accelerations applied via the ACEL command are available to be applied directly to the transient dynamic analysis.
Note: For consistent reaction forces, apply accelerations in the modal analysis rather than in the transient analysis.
Element loads (pressures, temperatures, accelerations, etc.) are not directly applied to the transient dynamic analysis, but loads that were applied in the preceding modal analysis can be transferred to the transient analysis via load vectors and the LVSCALE command. Use a zero scale factor on the LVSCALE command to suppress a load vector at a particular load step. If you use LVSCALE, ensure that all nodal forces (F) defined in the modal analysis solution are removed in the transient analysis. Generally, you should apply nodal forces in the transient part of the analysis.
If the transient excitation is coming from support motion and if you requested the pseudo-static modes in the modal analysis (MODCONT command), you can use the DVAL command to specify the enforced displacements and accelerations. Imposed nonzero displacements (D command) are ignored.
Multiple load steps are usually required to specify the load history in a transient analysis. The first load step is used to establish initial conditions, and second and subsequent load steps are used for the transient loading, as explained next.
Establish initial conditions. In modal superposition transient analyses, a first solution is done at TIME = 0. This establishes the initial condition and time step size for the entire transient analysis. Generally, the only load applicable for the first load step is initializing nodal forces. For more details, see Equation 15–40 in the Theory Reference. For this pseudo-static analysis, the mode-superposition method may yield poor results at TIME = 0 if nonzero loads are applied.
The following load step options are available for the first load step:
Dynamics options include the following:
Transient Integration Parameters (TINTP)
Transient integration parameters control the nature of the Newmark time-integration technique. The default is to use the constant average acceleration scheme with
GAMMA= 0.005; see your Mechanical APDL Theory Reference for further details.Damping
Damping in some form is present in most structures and should be included in your analysis. You can specify the following forms of damping in a mode-superposition transient dynamic analysis:
The only valid general option for the first load step is integration time step (DELTIM), which is assumed to be constant throughout the transient. By default, the integration time step is assumed to be 1/(20f), where f is the highest frequency chosen for the solution. The DELTIM command is valid only in the first load step and is ignored in subsequent load steps.
Note: If you do issue the TIME command in the first load step, it will be ignored. The first solution is always a static solution at TIME = 0.
The output control option for the first load step is printed output (OUTPR). Use this option to control printout of the nodal solution.
Specify loads and load step options for the transient loading portion.
General options include the following:
Output control options include the following:
The only valid label on these commands is NSOL (nodal solution). The default for OUTRES is to write the solution for every fourth time-point to the reduced displacement file. If you expanded element results during the modal analysis, then OUTRES is not applicable because the modal coordinates, not the displacements, are written to Jobname.rdsp.
By default, if you used the Block Lanczos, PCG Lanczos, Supernode, or Subspace option for the modal analysis (MODOPT,LANB; LANPCG; SNODE; or SUBSP), the modal coordinates (the factors to multiply each mode by) are written to the file Jobname.rdsp and no output controls apply. If however you explicitly request not to write the element results to the .mode file (MXPAND,,,,,,NO), the actual nodal displacements are written to the .rdsp file. In that case, you may use a nodal component with the OUTRES,NSOL command to limit the displacement data written to the reduced displacement file Jobname.rdsp. The expansion pass will only produce valid results for those nodes and for those elements in which all of the nodes of the elements have been written to the .rdsp file. To use this option, first suppress all writing by invoking OUTRES,NSOL,NONE, then specify the item(s) of interest by invoking OUTRES,NSOL,FREQ,component. Repeat the OUTRES command for any additional nodal components that you want to write to the .rdsp file. Only one output frequency is allowed. (The program uses the last frequency specified by OUTRES.)
Save a backup copy of the database to a named file.
Leave SOLUTION.
As an alternative method of resolution, you can issue the LSWRITE command to write each load step to a load step file (Jobname.S01) and then issue LSSOLVE to start the transient solution.
The mode-superposition transient solution (the modal coordinates) is written to the reduced displacement file, Jobname.rdsp, regardless of whether the Block Lanczos, PCG Lanczos, Supernode, Subspace, or QR damped method was used for the modal solution. Only the displacement, velocity, and acceleration solutions can be post-processed directly in POST26, and the modal coordinates can be plotted in POST1 using the PLMC command and listed using the PRMC command. For all other results (stress, forces, etc.), you will need to expand the solution.
The expansion pass starts with the transient solution on Jobname.rdsp and calculates the displacement, velocity, acceleration, stress, and force solutions based on OUTRES specifications. These calculations are performed only at the time points you specify. Before you begin the expansion pass, therefore, you should review the results of the transient solution (using POST26) and identify the critical time points.
Note: An expansion pass is not always required. For example, if your primary
interest is the displacement, velocity, or acceleration at specific points on
the structure, then the solutions on Jobname.rdsp could
satisfy your requirements. However, if you are interested in the stress or force
solution, then you must perform an expansion pass. Note that the velocity and
acceleration solutions need to be requested in the transient analysis
(VAout on the TRNOPT
command).
The .rdsp and .db files from the transient solution, along with the .mode, .emat, .esav and .mlv files from the modal solution must be available.
The full file (.full) must be available if linear acceleration (ACEL) is present in the mode-superposition analysis, or if coupling and/or constraint equations are present in the model, including constraint equations created during the solution by certain element types (contact elements, MPC184, and so on).
The residual force file (.resf) must be available if the residual response usage is activated (
KeyResp= ON on RESVEC).The database must contain the same model for which the transient solution was calculated.
The procedure for the expansion pass is explained below.
Reenter SOLUTION.
Command(s): /SOLUGUI:Activate the expansion pass and its options.
Option: Expansion Pass On/Off (EXPASS)
Select ON.
Option: Number of Solutions to be Expanded (NUMEXP)
Specify the number. This number of evenly spaced solutions will be expanded over the specified time range. The solutions nearest these times will be expanded. Also specify whether to calculate stresses and forces (default is to calculate both).
Option: Single Solution to Expand (EXPSOL)
Use this option to identify a single solution for expansion if you do not need to expand multiple solutions in a range. You can specify it either by load step and substep number or by time. Also specify whether to calculate stresses and forces (default is to calculate both).
Option: Residual Response Usage (RESVEC,,,,,ON)
If residual responses have been calculated during the modal analysis, you can add them to the expanded solution.
Specify load step options. The only options valid for a transient dynamic expansion pass are output controls:
Output Controls
Printed Output (OUTPR)
Use this option to include any results data on the output file (Jobname.out).
Note: If element results were calculated in the modal analysis, then no element output is available in the expansion pass. Use /POST1 to review the element results.
Database and Results File Output (OUTRES)
This option controls the data on the results file (Jobname.rst).
Extrapolation of Results (ERESX)
Use this option to review element integration point results by copying them to the nodes instead of extrapolating them (default).
Start expansion pass calculations.
Command(s): SOLVEGUI:Repeat steps 2, 3, and 4 for additional solutions to be expanded. Each expansion pass is stored as a separate load step on the results file.
Leave SOLUTION.
Command(s): FINISHGUI: Close the Solution window.
You review results for an expansion pass in the same way that you review results for most structural analyses. See Review the Results in "Structural Static Analysis".
You can review these results using POST1. (If you expanded solutions at several time points, you can also use POST26 to obtain graphs of stress versus time, strain versus time, and so on.) The procedure to use POST1 (or POST26) is the same as described for the full method.
Results consist of displacements, stresses, and reaction forces at each time-point
for which the solution was expanded. Results also include velocities and
accelerations when requested (VAout = YES on
TRNOPT). You can review these results using POST26 or POST1,
as explained for the full method (see Review the Results).
Note: By default, reaction forces and other force output (PRRSOL,
FSUM, RFORCE, etc.) contain only the
static contributions. The inertial and damping contributions are not included or
available (FORCE). If you want to obtain the inertial and
damping contributions, use VAout = YES on
TRNOPT to output the velocities and accelerations needed
for their calculation. If the element results are directly calculated from the
element modal results (MSUPkey = YES on
MXPAND), the element nodal loads must also be output
(OUTRES,NLOAD,ALL) at the modal analysis level.
If the results are calculated by combining the modal results
(MSUPkey = YES on MXPAND in
the modal analysis), some limitations apply. For more information, see Option: Number of Modes to Expand (MXPAND) in this guide.
Caution: The stiffness energy (SENE) and strain energy density (SEND) computed for a linear perturbation mode-superposition analysis with a nonlinear base analysis is an approximate solution and may not be accurate.
! Build the Model /FILNAM,... ! Jobname /TITLE,... ! Title /PREP7 ! Enter PREP7 --- ---! Generate model --- FINISH ! Obtain the Modal Solution /SOLU ! Enter SOLUTION ANTYPE,MODAL ! Modal analysis MODOPT,LANB ! Block Lanczos MXPAND,,,,YES ! Expand the results and calculate element results D,... ! Constraints SF,... ! Element loads ACEL,... SAVE SOLVE FINISH ! Obtain the Mode-Superposition Transient Solution /SOLU ! Reenter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,MSUP,... ! Mode-superposition method LVSCALE,... ! Scale factor for element loads F,... ! Nodal Loads MDAMP,... ! Modal damping ratios DELTIM,... ! Integration time step sizes SOLVE ! Solve 1st load step --- ! Remember: The 1st load step is --- ! solved statically at time=0. --- ---! Loads, etc. for 2nd load step TIME,... ! Time at end of second load step KBC,... ! Ramped or stepped loads --- SOLVE ! Solve 2nd load step (first transient load step) FINISH ! Review displacement results of the mode-superposition solution /POST26 ! Enter POST26 FILE,,RDSP ! Results file is Jobname.rdsp SOLU,... ! Store solution summary data NSOL,... ! Store nodal displacement result as a variable PLVAR,... ! Plot variables PRVAR,... ! List variables FINISH ! Expand the Solution /SOLU ! Reenter SOLUTION EXPASS,ON ! Expansion pass NUMEXP,... ! No. of solutions to expand; time range OUTRES,... ! Results-file data controls SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read desired set of results into database PLDISP,... ! Deformed shape PRRSOL,... ! Reaction loads PLNSOL,... ! Contour plot of nodal results PRERR ! Global percent error (a measure of mesh adequacy) --- ---! Other postprocessing as desired --- FINISH
See the Command Reference for discussions of the ANTYPE, MODOPT, ACEL, TRNOPT, LVSCALE, MDAMP, DELTIM, TIME, KBC, OUTRES, LSSOLVE, FILE, SOLU, NSOL, PLVAR, PRVAR, EXPASS, NUMEXP, OUTRES, PLDISP, PRRSOL, PLNSOL, and PRERR commands.