Response Dynamics – Setting up the FEM

Estimated time to complete: 20–30 minutes

Simcenter 3D Response Dynamics is an add-on to Pre/Post for use with Simcenter Nastran. It allows you to evaluate the dynamic responses of a structural model subjected to various loading conditions. The software calculates these responses using modal approaches.

The Response Dynamics tutorial focuses on evaluation of the dynamic displacements and stresses in a bracket used to support an electronics module in an engine compartment. It is divided into two activities:

  • Response Dynamics – Setting up the FEM: You prepare the simulation files and define the boundary conditions and solution options necessary for creating a solution process. You then solve the model and examine the normal modes.

  • Response Dynamics – Analyzing a transient event: You perform a transient analysis and review results.

For detailed information about the procedures and concepts discussed in this tutorial, see the

Response Dynamics section in the Pre/Post help.

1: Setup

  1. On your desktop or the appropriate network drive, create a folder named response.

  2. Click the link below:

    Download the part

  3. Extract the files to your response folder.

    Note:

    The response_functions.afu file contains two excitation functions. You will have the opportunity to create these functions as part of this tutorial; however, the completed functions are included for your convenience.

  4. Start Simcenter 3D or NX.

  5. Open rs_bracket_1_sim1.sim.

2: Reset dialog box memory

The options you select in dialog boxes are preserved for the next time you open the same dialog box within a given session. Restore the default settings to ensure that the dialog boxes are in the expected initial state for each step of the activity.

File

Preferences→User Interface

  • Options

  •   Reset Dialog Memory

  • OK

     
3: Create the response dynamics solution

  Simulation Navigator

  •  rs_bracket_1_sim1.sim

  •   New Solution

  •  

    Name

    Dynamics_Solution_1

  • Solver

    Simcenter Nastran

  • Analysis Type

    Structural

  • Solution Type

    SOL 103 Response Dynamics

     

    This is the modal analysis solution for Response Dynamics. You can also use the SOL 103 Real Eigenvalues solution, but loads are not considered.

  • OK

     
4: Specify solution result types

Specify the result types to recover in the solution. For this activity, you will recover stress, displacement, and acceleration.

  Simulation Navigator

  •     Dynamics_Solution_1

  •   Subcase – Dynamics

  •   Edit

  •   Edit (Output Requests)

  •  

    Acceleration

  •   Enable ACCELERATION Request

    Note:

    Stress and Displacement are enabled by default.

  • OK

     Structural Output Requests dialog box

Leave the Solution Step dialog box open for the next step.

5: Specify number of modes to generate

The Solution Step dialog box is open from the previous step.

  • Eigenvalue Method

    Lanczos

  •   Edit (Lanczos Data)

  • Frequency Range – Lower Limit

    0

  • Number of Desired Modes

    10

  • OK

     both dialog boxes

    This combination of a lower limit, no upper limit, and a number of desired modes means the solver will calculate the lowest-frequency modes within the number of modes desired, starting from the specified lower limit.

    Increasing the number of modes results in a more accurate representation of the structure, but also increases the solution time. You should include enough modes to cover your frequency range of interest.

6: Add the constraint to the solution

  Simulation Navigator

  •     Constraint Container

  •   UserDefined(1)

  •   Add to active solution or step

    The constraint is added to the Constraints container for the solution.

7: Add an enforced motion location

Add an enforced motion location to the top edge of the back face. These enforced degrees of freedom will trigger the generation of constraint modes when you solve the model. Later, you will apply an enforced motion excitation to these enforced degrees of freedom.

  Simulation Navigator

  •   Dynamics_Solution_1

  •   Constraints

  •   New Constraint→Enforced Motion Location

  • Method (Top Border bar)

    Feature Edge Nodes

  •   an element edge along the top edge of the bracket

    All nodes along the edge are selected.

  • DOF3

    Enforced

  • OK

     
8: Solve the response dynamics solution

Now you are ready to solve the response dynamics solution and generate the modes.

  Simulation Navigator

  •   Dynamics_Solution_1

  •   Solve

  • OK

     

  • Wait until the solution is complete.

  • No

     Review Results dialog box

  •   the Information window

  • Cancel

     Analysis Job Monitor dialog box

9: Create the Response Dynamics solution process

  (hover over the tabbed area of the Top Border bar with the mouse)

  •   Response Dynamics (select, if necessary)

 

Response Dynamics

  New Response Dynamics (Response Dynamics group)

  • Name

    RS_Meta_Solution_1

  • OK

     

Notice the nodes that appear in the Simulation Navigator.

RS_Meta_Solution_1
Dynamics_Solution_1
Modal Representation
Normal Modes [10]
Constraint Modes [15]
Attachment Modes [0]
Sensors
Strain Gages

  Save

10: Quick View the mode shapes

  Simulation Navigator

  •   Normal Modes [10] (under the RS_Meta_Solution_1 node)

  •  

     
    Note:

    If the Response Dynamics Details View is not visible, click the bar at the bottom of the Simulation Navigator to open it.

    This panel displays the dynamic characteristics (frequency, mass, damping, and stiffness) for each normal mode solved in the response dynamics solution.

    The modal representation for this model consists of 10 normal modes and 15 constraint modes. Each enforced DOF in the enforced motion location you defined earlier generated a single constraint mode. Your enforced motion location has 15 nodes with one DOF enforced, so 15 constraint modes were generated.

  •   Normal Modes [10]

  •   Quick View

    By default, displacement magnitude results for Mode 1 are displayed.

 

Results

  Next Mode/Iteration (Quick Edit group)

Use the Next Mode/Iteration command to view additional modes.

  Return to Model (Context group)

11: Apply viscous damping to the normal modes

Home

  Simulation Navigator

  •   Normal Modes [10] (under the RS_Meta_Solution_1 node)

  •   Edit Damping Factor

  • Viscous

    4.0

  • Enter

     

  • OK

     

  •  

     

  • Compare the values in the Frequency column to the values in the Damped Frequency column.

    Because you applied the command to the Normal Modes node, the software applies the damping to all ten modes. You can define damping for individual modes by right-clicking the mode in the Response Dynamics Details View panel and choosing Edit Damping Factor.

12: Deactivate irrelevant modes

  Normal Modes [10] (under the RS_Meta_Solution_1 node)

In the Response Dynamics Details View panel, note the mass values of each mode in the Z direction (under the %Z_Mass column).

In this simple scenario, you are interested only in the dynamic response in the Z-direction. As a general rule, you should have at least 80% representation of mass in the direction you are evaluating to achieve an accurate analysis. Modes 1, 3, and 7 are the only significant modes in the Z-direction. (In general, you can consider modes that contribute more than 0.5% to be significant.) Together, they represent 95.8% of the mass in the Z-direction.

Note:

The columns in the picture have been rearranged for clarity.

The values that you see in your model may be slightly different.

To further reduce the modal model, you can remove modes 2, 4, 5, 6, 8, 9, and 10 from the analysis because they do not contribute to the modal mass in the direction of interest.

Modes with an asterisk character (*) in the # Mode column are considered “active” in your response evaluations. By default, all modes are marked as active.

Ctrl

 + modes 2, 4, 5, 6, 8, 9, and 10

  Deactivate

The asterisk characters next to the selected modes disappear.

  Save

13: Evaluate transmissibility

Transmissibility is a frequency response function that lets you evaluate the response of one or several output nodes to an enforced motion input such as displacement, velocity, or acceleration at a selected node.

  Simulation Navigator

  •   RS_Meta_Solution_1

  •   Evaluate Transmissibility

  • Result

    Displacement

  • Input Motion Type

    Acceleration

  •   Excitation Location List (ID)

  • Select Excitation Location

    Node[number]: Z

    Select an ID number in the Select Excitation Location dialog box that corresponds to a node near the center of the top edge of the back face. The node that you select is highlighted in the graphics window (see below). Because you will need to know the ID number of this node later in this activity, write it down.

    Note:

    The ID number in your model will be different from that shown in the illustration.

  • OK

     Select Excitation Location dialog box

  •  

     

  • Data Component

    Z

    Note:

    Z is the only selectable direction because your enforced motion location was defined in the Z direction.

Note:

You cannot use the Evaluate FRF command because FRF evaluates frequency response to a unit force load, and, in this case, the load point is grounded with the enforced motion location constraint. You cannot use the same model to apply a force and displacement (or acceleration) to the same node.

Leave the Evaluate Transmissibility dialog box open for the next step.

14: Specify output nodes

The Evaluate Transmissibility dialog box is still open from the previous step.

  •  

  •   Node (Select Node)

  •   (the two opposite corner nodes and the CONM2 element)

  •  

     

  • Data Component

    Z

Leave the Evaluate Transmissibility dialog box open for the next step.

15: Specify frequency range

The Evaluate Transmissibility dialog box is still open from the previous step.

  •  

  •   Range (Method)

  • Frequency Start Value

    0

  • Frequency End Value

    40

    This frequency range should cover the frequency of the 3 active normal modes.

  • OK

     

  •   Create New Window (Viewport dialog bar)

  • Notice the first peak in the graph; it is the zero-frequency response. But because of the frequency increment, it does not appear at 0 Hz. In the next step, you will fix this issue.

  •   Graph Window 1

16: Add spectral lines

Increase the resolution of the graph by adding spectral lines.

Repeat the previous steps to evaluate transmissibility.

  • Select the same enforced motion location and output nodes that you used in the previous steps, and use the same values in the Evaluate Transmissibility dialog box (which should be preserved from the previous steps).

  • Additional Spectral Lines

    1000

  • OK

     

  •   Create New Window (Viewport dialog bar)

  •   Graph Window 1

  Save

This step concludes the first Response Dynamics tutorial. If you plan to continue now with the Response Dynamics – Analyzing a transient event tutorial, leave the Simulation file open. Otherwise, retain the files from this completed activity because you will need them for the next tutorial.