Because this analysis is linked to (or based on) modal responses, a Modal analysis is a prerequisite. This setup allows the two analysis systems to share resources such as engineering data, geometry and boundary condition type definitions made in modal analysis.

---

Note:

• When you set the Solution Method property to Mode Superposition (MSUP), the harmonic analysis can be linked to a pre-stressed modal analysis.

• When solving a linked MSUP harmonic system database from a version prior to the most current version of Mechanical, it is possible to encounter incompatibility of the file file.full created by the modal system. This incompatibility can cause the harmonic system’s solution to fail. In the event you experience this issue, use the Clear Generated Data feature and resolve the modal system.

  Refer to the Obtain the Mode Superposition Harmonic Solution section of the MAPDL Structural Analysis Guide for more information.

---

From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Harmonic Response template directly onto the Solution cell of the Modal template.

---

Note:  You can create a modal environment in a Harmonic Response system that is already open in Mechanical by:

1. Selecting the Modal option from the Analysis drop-down menu on the Home (or displayed) tab.

2. Setting the Modal Environment property (of the Pre-Stress/Modal object) to the Modal system.

---

For this analysis configuration, the basic Analysis Settings include:

Step Controls

This category enables you to define step controls for an analysis that includes rotational velocities in the form of revolutions per minute (RPMs). You use the properties of this category to define RPM steps and their options. Each RPM load is considered as a load step, such as frequency spacing, minimum frequencies, maximum frequencies, etc.

The Step Controls category enables you to define step controls for an analysis that includes multiple load steps. You use the properties of this category to define the load steps and their options. When you select the Analysis Settings object, the content of the Step Controls category automatically displays in the Worksheet. You can modify certain properties in either the Worksheet or in the Details pane. For each load step, you can specify solution settings (Frequency Spacing, minimum frequencies, maximum frequencies, etc.). See the Step Controls for Harmonic Analysis Types section for a description of the properties.

Options

See the Harmonic Analysis Options Group section for a complete listing of the Details properties for a Harmonic Response analysis. Note that for a Harmonic Analysis Using Linked Modal Analysis System, only the Mode Superposition option is applicable for the Solution Method property and it is therefore read-only.

In addition, you can turn on the following properties:

• Include Residual Vectors. Set this property to Yes to execute the RESVEC command and calculate residual vectors.

• Cluster Results: Set this property to Yes to automatically cluster solution points near the structure’s natural frequencies ensuring capture of behavior near the peak responses. This results in a smoother, more accurate, response curve.

• On Demand Expansion Option: Options for this property include Program Controlled (default), Yes, and No. When set to Program Controlled, an additional read-only property, On Demand Expansion, displays. This property only displays for the Program Controlled option and the application determines the value for the property, either Yes or No.

  When the On Demand Expansion Option property is set to Yes, either manually or from the Program Controlled setting, the application creates the result file optimally. The application evaluates the results using the Modal solution data and calculates any other results “on demand.” This improves solution performance and reduces file size. In addition, the application automatically removes mode shape data from the result file as determined by the On Demand Mode Shape preference.

  You can change the default setting for the On Demand Expansion Option property and the On Demand Mode Shape preference using the Options (Modal, Harmonic and Transient Mode Superposition) category of the Analysis Settings and Solution group in the Options dialog.

• Mode Selection Method: This property enables you to select the modes for the mode expansion. Property options include:

  • None (default): This option expands all the extracted modes from the modal analysis. All the modes participate in the Mode Superposition harmonic analysis.

  • Modal Effective Mass: When you select this option, the Significance Threshold property also displays. For the Significance Threshold property value, the application selects the modes that have a ratio for the Modal Effective Mass to the Total Mass that is greater than this value, in all directions, for expansion. That is, only the selected modes participate in the Mode Superposition harmonic response analysis. The application default is 0.001. This feature improves the performance of postprocessing the modal results and reduces the file size.

Also, Mode Frequency Range is not applicable because available modes are defined in the linked Modal system.

---

Note:  The following boundary conditions do not support residual vector calculations:

• Nodal Force

• Remote Force scoped to global a Remote Point (created via Model object)

• Moment scoped to global a Remote Point (created via Model object)

---

Output Controls

This category enables you to request Stress, Strain, Nodal Force, and Reaction results to be calculated. For better performance, you can also choose to have these results expanded from Harmonic or Modal solutions. To expand reaction forces in the modal solution, set the Nodal Force property to Yes or Constrained Nodes.

You must specify the desired upstream Modal analysis in the Modal Environment property of the Initial Conditions object for the Harmonic Response analysis. This object also indicates whether the upstream Modal analysis is pre-stressed. If it is a pre-stress analysis, the name of the pre-stress analysis system is displayed in the Pre-Stress Environment property, otherwise the field indicates None. The Modal analysis must extract enough modes to cover the frequency range. A conservative estimate is to extract enough modes to cover 1.5 times the maximum frequency in the excitation.

---

Note:

• Command objects can be inserted into Initial Conditions object to execute a restart of the solution process for the Modal Analysis.

• If displacement loading is defined with Displacement, Remote Displacement, or Bolt Pretension (specified as Lock, Adjustment, or Increment) loads in the Static Structural analysis, these loads become fixed boundary conditions for the Harmonic solution. This prevents the displacement loads from becoming a sinusoidal load during the Harmonic solution.

---

The following loads are allowed for the linked analysis:

Inertial

Acceleration (Phase Angle is not supported.)

Loads

• Acceleration as a base excitation

• Bearing Load (Phase Angle is not supported.)

• Given a specified Displacement

• Force (applied to a face, edge, or vertex)

• Line Pressure

• Moment

• Pressure

• Pipe Pressure (line bodies only)

• Remote Force

Direct FE

The Direct FE option Nodal Force is supported for node-based Named Selection scoping and constant loading only.

---

Note:

• For the Force and Pressure loading conditions, the default setting for the Applied By property is Direct.

• When you have a supported topology (geometric or mesh entity) selected on your model, and you insert a Remote Force or a Moment, the application automatically creates (promotes) a corresponding Remote Point for the specified load and scopes the load to that Remote Point. This promotion feature is only available when none of the analyses in your project have been solved.

---

Loading and Support Limitations

Note the following load and support requirements and limitations:

• Remote Force is not supported for vertex scoping.

• Moment is not supported for vertex scoping on 3D solid bodies because a beam entity is created for the load application.

• During a linked MSUP Harmonic analysis, if a Remote Force or Moment scoped to an internal remote point is specified with the Behavior property set to Deformable, the boundary conditions cannot be scoped to the edges of line bodies such that all of their nodes in combination are collinear.

• The Force Reaction and Moment Reaction probes are not supported for a either a Harmonic Response analysis or a Transient structural analysis using the Mode Superposition method Solution Method when 1) the Damping Ratio property is defined with a non-zero value and 2) if the Analysis Settings property Expand Result From is set to Harmonic Solution or Transient Solution.

Refer to the Review Results topic in the Harmonic Response Analysis section for more information regarding how to set up the harmonic results.