Because this analysis is linked to (and based on) structural responses, a Static-Structural analysis is a prerequisite. This setup allows the two analysis systems to share resources, such as engineering data, geometry, and the boundary condition type definitions that are defined the in the structural analysis.

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

---

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

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

2. Setting the Pre-Stress Environment property (of the Pre-Stress object) to the Static Structural system.

---

For this analysis configuration, the basic Analysis Settings include:

Step Controls

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 Options for harmonic analyses section for a complete listing of the properties. For a harmonic response analysis linked to an upstream static structural analysis, Mode Superposition is not an available selection.

Output Controls

You can specify This category enables you to request Stress, Strain, Nodal Force, and Reaction results to be calculated.

The Initial Conditions (Pre-Stress) object of the Harmonic Response analysis must point to the linked Static Structural analysis.

---

Note:

• All structural loads, including Inertial loads, such as Acceleration and Rotational Velocity, are deleted from the Harmonic Analysis portion of the simulation once the loads are applied as initial conditions (via the Pre-Stress object). Refer to the Mechanical APDL command PERTURB,HARM,,,DZEROKEEP for more details.

• For Pressure boundary conditions in the Static Structural analysis: if you define the load with the Normal To option for faces (3D) or edges (2-D), you could experience an additional stiffness contribution called the "pressure load stiffness" effect. The Normal To option causes the pressure acts as a follower load, which means that it continues to act in a direction normal to the scoped entity even as the structure deforms. Pressure loads defined with the Components or Vector options act in a constant direction even as the structure deforms. For a same magnitude, the "normal to" pressure and the component/vector pressure can result in significantly different results in the follow-on Full-Harmonic Analysis. See the Pressure Load Stiffness topic in the Applying Pre-Stress Effects for Implicit Analysis Help Section for more information about using a pre-stressed environment.

• If displacement loading is defined with Displacement, Remote Displacement, Nodal 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. If you define a Nodal Displacement in the Harmonic analysis at the same location and in the same direction as in the Structural Static analysis, it overwrites the previous loading condition and/or boundary condition in the Harmonic solution.

---

The following loads are allowed for linked Harmonic Response (Full) analysis:

• Inertial: Acceleration (Phase Angle is not supported.)

• Direct FE (node-based Named Selection scoping and constant loading only):

  • Nodal Force

  • Nodal Pressure (Phase Angle is not supported.)

  • Nodal Displacement - At least one non-zero Component is required for the boundary condition to be fully defined.

---

Note:  Any other boundary conditions must be defined in the prerequisite (parent) Structural Analysis, such as Support Type boundary conditions.

---