(800) 566-9190 Contact Us Follow SimuTech Group on LinkedIn Follow SimuTech Group on Facebook SimuTech Group’s Twitter account SimuTech Group’s YouTube Channel

SimuTrain® is ANSYS training on demand!

  • Basic & Advanced Level Training Modules
  • ANSYS & SimuTech Training Videos
  • Lectures, Tutorials & Workshops
  • 1 hour Web-based ANSYS Sessions to Practice Hands-on Workshops

Learn more about SimuTrain or get started today by purchasing your subscription.


Follow SimuTech Group on LinkedIn Follow SimuTech Group on Facebook Follow SimuTech on Twitter SimuTech Group’s YouTube Channel

Harmonic Analysis Face Rotation Measurement in ANSYS® Workbench Mechanical

ANSYS Harmonic Face Rotation 1

Figure 1: Harmonic Load on the End of a Cantilevered Plate


ANSYS Workbench Mechanical can perform harmonic response analysis, by either modal superposition, or by full harmonic analysis. Measurement of face rotation is sometimes of interest to customers. If a remote point is associated with a face of interest, rotation of that remote point can be measured in an APDL Commands Object, and reported to the user, with the option of creating an output parameter from the rotation value.

In Figure 1 above, the far end of a plate has been fixed. The nearer end has harmonic loads applied at two edges, one pointing up, and one pointing down. The objective is to excite the plate at frequencies around a mode of vibration that has the twisting motion implied by these forces.

End face rotation will be measured, using a Remote Point that is associated with the face, and set to “Deformable” so that the behavior of the model is not influenced. Associating a remote point with a face meshed with a large number of nodes can increase solution time and memory requirement—setting a pinball radius can reduce this.

Recent features in ANSYS that make it easier to find amplitude results in harmonic analysis are illustrated here. Settings that measure face rotation in harmonic analysis will be reviewed.

Details of Rotation Measurement in a Harmonic Response Analysis

In the Workbench project page, a modal analysis can be linked to a subsequent harmonic response analysis:

ANSYS Harmonic Face Rotation 2

Figure 2: Linked Modal and Harmonic Response Analyses

The modal analysis can be helpful before a harmonic run in order to discover at what frequencies a structure may respond substantially to an excitation. If a modal analysis has included enough frequencies to more than cover the range of excitation frequencies in a harmonic response analysis, then modal superposition can be used in the harmonic response analysis, as an alternative to full harmonic response analysis.

If Figure 3 below, it can be seen that the second mode involves rotation of the free end of the cantilever plate around the Z axis, at a frequency of 6097.1 Hz. Note: the predicted frequency can be sensitive to the mesh density.

ANSYS Harmonic Face Rotation 3

Figure 3: Second Mode of Vibration in a Cantilever Plate 

In Figure 4 below a Remote Point has been created and automatically positioned at the centroid of the end face on the plate. All degrees of freedom are active, and the associated face is set to the default “Deformable” so that it can flex as if the Remote Point was not there.

ANSYS Harmonic Face Rotation 4

Figure 4: Remote Point at Centroid of Face Set to Deformable

An APDL Commands Object can be inserted for the Remote Point, and used to remember the number of the node assigned to the remote point. The variable “Measure_Pilot” is created for this purpose, as seen below in Figure 5

ANSYS Harmonic Face Rotation 5

Figure 5: APDL Command Remembers Pilot Node Number at Remote Point

Here is the APDL command:


In Figure 6 below, a Harmonic Response has Analysis Settings input to indicate a range of frequencies of interest, and the number of intervals between frequencies to be analyzed:

ANSYS Harmonic Face Rotation 6

Figure 6: Analysis Settings for a Harmonic Sweep between 5900 and 6300 Hz

With loading as described in Figure 1, the amplitude of Y displacement calculated at 6096 Hz can be displayed as in Figure 7 below, at a frequency close to resonance:

ANSYS Harmonic Face Rotation 7

Figure 7: Amplitude of Vertical Displacement Y at 6096 Hz

Insight as to the peak response around a resonant frequency can be obtained in a Frequency Response plot set to show Amplitude, as below in Figure 8 for a vertex at a corner of the free face of the plate:

ANSYS Harmonic Face Rotation 8

Figure 8: Frequency Response--Amplitude of Vertex Y Movement across the Range of Frequencies

Further insight results from a phase plot for the vertex, as in Figure 9. Note the phase angle near resonance:

ANSYS Harmonic Face Rotation 9

Figure 9: Phase Angle Response—Phase Angle of Vertex Y Movement across the Range of Frequencies

The frequency and phase angle as seen above in Figure 8 and Figure 9 can be used to obtain a directional deformation plot in which the values are not absolute values. Since the phase angle is entered for the frequency, we see in Figure 10 the magnitude of the displacement without the absolute value being assigned:

ANSYS Harmonic Face Rotation 10

Figure 10: Y Displacement at Vertex at 6096 Hz and Phase Angle -88.795

An APDL Commands Object can be used to load a result of interest, and read the amplitude of vibration at a remote point. This is illustrated in Figure 11, using the node number recorded in Figure 5:

ANSYS Harmonic Face Rotation 11

Figure 11: APCL Commands Object to Measure Rotation of Pilot Node at Specified Substep, Implying Frequency 

Here are the APDL commands used in Figure 11 above to measure and report the rotations about the X, Y and Z axes. In this example, the user provides the substep number that corresponds to the frequency of interest. Users must remember to request Amplitude in the SET command:

/com, *
/com, *******************************************
/com, *******************************************
/com, *******************************************
/com, *
/com, Check rotation result
set,1,49,,AMPL                            ! want amplitude
*get,my_freq,ACTIVE,,SET,FREQ             ! what frequency was read
/com, *
/com, *******************************************
/com, *******************************************
/com, *******************************************
/com, *

Note that the SET command above could directly request a frequency with the Time argument:

SET, Lstep, Sbstep, Fact, KIMG, TIME, ANGLE, NSET, ORDER

Result check: Divide vertical movement (left - right vertex) by width and rotation is estimated:

ATAN(2*0.04893/39.975) = 0.14026 degrees

This angle is close to that of the remote point in Figure 11, which considers all of the nodes on the face.


Workbench Mechanical can be used to perform a Harmonic Response dynamic analysis. A remote point can be created, and used in APDL commands to measure a rotation angle amplitude at a frequency of interest.

A modal analysis is often performed prior to another dynamic analysis in order to characterize the system of interest. Because a harmonic response analysis is linear, modal superposition can be used if desired, as long as enough modes are extracted to more than cover the range of harmonic excitation frequencies.

Plots of frequency response and phase response can augment an understanding of a harmonic response analysis. For user convenience, recent ANSYS versions permit direct measurement of amplitude of a harmonic response, without going through combinations of real and imaginary components, or of phase and amplitude.

This article illustrates APDL commands that can return rotation angle at a chosen frequency.

Looking for more ANSYS Tips & Tricks?

Check out 300+ more videos and articles on our SimuTrain® Portal.

Get SimuTrain Now!