The mode-superposition method sums factored mode shapes (obtained from a modal analysis) to calculate the harmonic response. The procedure to use the method consists of five main steps:
Also see Example: Mode-Superposition Harmonic Analysis.
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, QR damped, or Unsymmetric. (Other methods do not apply to mode-superposition.)
If damping and/or an unsymmetric stiffness or damping matrix is present, use the QR Damp mode-extraction method (MODOPT,QRDAMP) and do not request the calculation of the complex eigenmodes (
Cpxmod= OFF on MODOPT).If your model is undamped with an unsymmetric stiffness and/or mass matrix, use the unsymmetric mode-extraction method (MODOPT,UNSYM) and request both left and right modes (
ModType= BOTH on MODOPT).Extract all modes that may contribute to the harmonic response.
If using 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.
To apply harmonically varying element loads (such as pressures, temperatures,or accelerations), specify them in the modal analysis. The program ignores the loads for the modal solution, but calculates a load vector and writes it to the mode shape file (Jobname.mode) and also writes the element load information to the Jobname.mlv file. You can generate multiple load vectors (see the MODCONT command in Generating and Using Multiple Loads in Mode-Superposition Analyses). The load vectors created can then be scaled and used in the harmonic solution.
To include the contribution of higher frequency modes in the subsequent harmonic 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 harmonic excitation is coming from the support, you can generate pseudo-static modes needed in the subsequent harmonic analysis (see the MODCONT command in Enforced Motion Method for Mode-Superposition Transient and Harmonic Analyses).
To save computation time in the subsequent expansion of the harmonic results, expand the modes and calculate the element results (MXPAND,ALL,,,YES,,YES). Do not use this option if you are applying thermal loads; see Option: Number of Modes to Expand (MXPAND) for details about this limitation. If you want to postprocess total reaction forces, output element nodal loads (OUTRES,NLOAD,ALL) .
Do not change the model data (for example, nodal rotations) between the modal and harmonic analyses.
You can select the modes of interest for the expansion. Because the expansion is performed on the selected modes only, you will save computational time in the subsequent mode-superposition harmonic analysis. See Using Mode Selection for information about the 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 harmonic response. The following requirements apply:
The mode shape file (Jobname.mode) must be available.
If the unsymmetric eigensolver is used, the left mode shape file (Jobname.lmode) must also be available (
ModType= BOTH on the MODOPT command). Unlike the Jobname.mode file which contains participation factors, load vectors, and other information, the Jobname.lmode file only contains the left eigensolutions.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 from 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.
Enter the solution processor (/SOLU).
Define the analysis type and analysis options. These are the same as described for the full method, except for the following differences:
Select the mode-superposition method of solution (HROPT).
Specify the modes you want to use for the solution (HROPT). This determines the accuracy of the harmonic solution. Generally, the number of modes specified should cover about 50 percent more than the frequency range of the harmonic loads.
To include the contribution of higher frequency modes, add the residual vectors calculated in the modal analysis (RESVEC,ON).
Optionally, cluster the solutions about the structure's natural frequencies (HROUT) for a smoother and more accurate tracing of the response curve.
Optionally, at each frequency, print a summary table that lists the contributions of each mode to the response (HROUT). Note, OUTPR,NSOL must be specified to print mode contributions at each frequency.
Apply loads on the model. Harmonic loading is the same as described for the full method, except for the following restrictions:
Only nodal forces (F, FK) and accelerations applied via the ACEL command are available to be applied directly to the harmonic analysis.
Note: You should apply accelerations in the modal analysis rather than in the harmonic analysis in order to obtain consistent reaction forces.
Element loads (pressures, temperatures, accelerations, etc.) are not directly applied to the harmonic analysis, but loads that were applied in the preceding modal analysis can be transferred to the harmonic 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. Note that ALL loads from the modal analysis are scaled, including forces and accelerations. To avoid load duplication, delete any loads that were applied in the modal analysis.
If the harmonic excitation is coming from support motion and 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.
Specify load step options.
You can request any number of harmonic solutions to be calculated (NSUBST). The solutions (or substeps) will be evenly spaced within the specified frequency range (HARFRQ). For example, if you specify 10 solutions in the range 30 to 40 Hz, the program will calculate the response at 31, 32, 33, ..., 39, and 40 Hz. No response is calculated at the lower end of the frequency range.
For the cluster option, the NSUBST command specifies the number of solutions on each side of a natural frequency if the clustering option (HROUT) is chosen. The default is to calculate four solutions, but you can specify any number of solutions from 2 through 20. (Any value over this range defaults to 10 and any value below this range defaults to 4.)
You can also directly define forcing frequencies using the
FREQARRandTolerinputs on the HARFRQ command. These user-defined frequencies are merged to the frequencies calculated with the previous options, if any.Damping in some form should be specified; otherwise, the response will be infinity at the resonant frequencies. ALPHAD and BETAD result in a frequency-dependent damping ratio, whereas DMPRAT specifies a damping ratio to be used at all frequencies. MDAMP specifies a damping ratio for each individual mode. DMPSTR specifies a constant structural damping coefficient. See Damping for further details.
By default, if you used the Block Lanczos, PCG Lanczos, Supernode, Subspace, or unsymmetric option for the modal analysis (MODOPT,LANB; LANPCG; SNODE; SUBSP; or UNSYM), the modal coordinates (the factors to multiply each mode by) are written to the file Jobname.rfrq and no output controls apply. If however you explicitly request not to write the element results to the Jobname.mode file (MXPAND,,,,,,NO), the actual nodal displacements are written to the .rfrq 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.rfrq. 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 .rfrq 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,ALL,component. Repeat the OUTRES command for any additional nodal components that you want to write to the .rfrq file.
Save a copy of the database (SAVE).
Start solution calculations (SOLVE).
Repeat steps 3 to 7 for any additional loads and frequency ranges (that is, for additional load steps). If you plan to do time-history postprocessing (POST26), the frequency ranges should not overlap from one load step to the next.
Leave SOLUTION (FINISH).
The mode-superposition harmonic solution (the modal coordinates) is written to the reduced displacement file, Jobname.rfrq, regardless of whether the Block Lanczos, PCG Lanczos, Supernode, Subspace, QR damped, or unsymmetric method was used for the modal solution. The displacement solution 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 harmonic solution on Jobname.rfrq and calculates the displacement, stress, and force solution. These calculations are done only at frequencies and phase angles that you specify. Therefore, before you begin the expansion pass, you should review the results of the harmonic solution (using POST26) and identify the critical frequencies and phase angles.
An expansion pass is not always required. For instance, if you are interested mainly in displacements at specific points on the structure, then the displacement solution could satisfy your requirements. However, if you want to determine the stress or force solution, then you must perform an expansion pass.
The .rfrq and .db files from the harmonic solution, and 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 left modes file (.lmode) must be available if the unsymmetric method (MODOPT,UNSYM) is used and both left and right eigenvectors are requested (
ModType= BOTH).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 harmonic solution was calculated.
The procedure for the expansion pass follows:
Reenter the solution processor (/SOLU).
Activate the expansion pass and its options. Mechanical APDL offers these options for the expansion pass:
Each of these options is explained in detail below.
Option: Expansion Pass On/Off (EXPASS)
Select ON.
Option: Number of Solutions to Expand (NUMEXP,NUM)
Specify the number. This number of evenly spaced solutions will be expanded over a frequency range (specified next). For example, NUMEXP,4,1000,2000 specifies four solutions in the frequency range 1000 to 2000 (that is, expanded solutions at 1250, 1500, 1750, and 2000).
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 frequency. Also specify whether to calculate stresses and forces (default is to calculate both).
Option: Phase Angle for Expansion (HREXP)
If multiple solutions are to be expanded over a frequency range (NUMEXP), we suggest that you request both the real and imaginary parts to be expanded (HREXP,ALL). This way, you can easily combine the two parts in POST26 to review the peak values of displacements, stresses, and other results.
If, on the other hand, a single solution is to be expanded (EXPSOL), you can specify the phase angle at which peak displacements occurred using HREXP,angle.
Option: Stress Calculations On/Off (NUMEXP or EXPSOL)
You can turn off stress and force calculations if you are not interested in them. Default is to calculate stresses and forces.
Option: Nodal Solution Listing Format (HROUT)
Determines how the harmonic displacement solution is listed in the printed output (Jobname.out). You can choose between real and imaginary parts (default), and amplitudes and phase angles.
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 harmonic expansion pass are output controls:
Printed Output (OUTPR)
Use this option to include any results data on the printed output file (Jobname.out). Note that if the element results were calculated in the modal analysis, then no element output is available in the expansion pass. Use /POST1 to review element results.
Database and Results File Output (OUTRES)
Use this option to control 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). Note that if the element results were calculated in the modal analysis, then this option is not applicable
Start expansion pass calculations (SOLVE).
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 the solution processor (FINISH). You can now review results in the postprocessor.
Results consist of displacements, stresses, and reaction forces at each frequency point for which the solution was expanded. You can review these results using POST26 or POST1, as explained for the full method (see Reviewing the Results).
The only POST1 (or POST26) procedure difference between this method and the full method is that if you requested expansion at a specific phase angle (HREXP, angle) there is only one solution available for each frequency. Use the SET command to read in the results.
If 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).
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 and calculate element results D,... ! Constraints SF,... ! Element loads SAVE SOLVE ! Initiate modal solution FINISH ! Obtain the Mode-Superposition Harmonic Solution /SOLU ! Enter SOLUTION ANTYPE,HARMIC ! Harmonic analysis HROPT,MSUP,... ! Mode-superposition method; number of modes to use HROUT,... ! Harmonic analysis output options; cluster option LVSCALE,... ! Scale factor for loads from modal analysis F,... ! Nodal loads HARFRQ,... ! Forcing frequency range DMPRAT,... ! Damping ratio MDAMP,... ! Modal damping ratios NSUBST,... ! Number of harmonic solutions KBC,... ! Ramped or stepped loads SAVE SOLVE ! Initiate solution FINISH ! Review the Results of the Mode-Superposition Solution /POST26 FILE,, ! Postprocessing file is Jobname.rfrq NSOL,... ! Store nodal result as a variable PLCPLX,... ! Define how to plot complex variables PLVAR,... ! Plot variables FINISH ! Expand the Solution (for Stress Results) /SOLU! Re-enter SOLUTION EXPASS,ON ! Expansion pass EXPSOL,... ! Expand a single solution HREXP,... ! Phase angle for expanded solution SOLVE FINISH ! Review the Results of the Expanded Solution /POST1 SET,... ! Read results for desired frequency PLDISP,... ! Deformed shape PLNSOL,... ! Contour plot of nodal results --- FINISH
See the Command Reference for a discussion of the ANTYPE, MODOPT, HROPT, HROUT, LVSCALE, F, HARFRQ, DMPRAT, DMPSTR, MDAMP, NSUBST, KBC, FILE, NSOL, PLCPLX, PLVAR, EXPASS, EXPSOL, HREXP, SET, and PLNSOL commands.