TAM Development

Modal testing requires installing instrumentation on a test article to accurately measure all of the relevant modes of a structure. Pretest analysis is the process of identifying the degrees of freedom required to accurately capture the mass and stiffness properties of a Finite Element Model (FEM).

The six steps to performing pretest analysis are defined below.

Steps:

  1. Build FEM and Solve for Modes
  2. Define Target Modes
  3. Select Test DOF (ASET)
  4. Build Test Display Model
  5. Generate TAM Matrices in NASTRAN
  6. Load TAM matrices using IMAT functions and Verify Pretest Analysis

 

It is important to note that Steps 3, 4, 5, and 6 do not happen sequentially; rather, they all occur somewhat in parallel. The process is iterative and many changes may be made throughout the process. An initial test instrumentation set, know as the ASET, gives shape to an initial test display model. This information is used to generate the first TAM matrix which is loaded into IMAT and used to verify whether the selected DOF are sufficient to capture the target modes of the test article. There are many ways to select an ASET, including GA (insert hyperlink).

 

Step 1 - Build FEM and Solve for Modes

IMAT users doing pretest analysis should be familiar with NASTRAN and how to perform a standard modal solution (solution 103).

 

Step 2 - Define Target Modes

As with Step 1, IMAT users should be able to identify mode shapes that they feel are important for their test. This can be done a number of different ways:

 

Step 3 - Select Test DOF

Selecting the test DOF is something that varies from project to project. Generally, this step is an iterative process involving intuition. A good rule of thumb for the number of accelerometers required for a test is 10x the number of target modes. Using the Genetic Algorithm or selectASET it is possible to develop an instrumentation set that requires only 3-4x the number of accelerometers as there are target modes. Please refer to GA's and selectASET's documentation for more information about using these methods.

After an initial set of DOF are selected, an orthogonality or MAC criterion is used to determine if the selected DOF sufficiently represent the target modes. In order to calculate orthogonality, however, you must first develop a TAM mass matrix as detailed in Step 5. The orthogonality checking process is then described in Step 6. Therefore steps 3, 5, and 6 are taken together and repeated several times throughout the pretest process.

 

Step 4 - Build the Test Display Model

The objective of building a test display model is to help the test engineer visualize structure deformation, such as mode shapes, using a subset of the nodes comprising the complete finite element model. Back expansion is the process where the measured degrees of freedom are used to approximate the motion of unmeasured degrees of freedom, using the FEM stiffness matrix. One common usage of a back-expansion matrix is to fill in the missing DOF of a non-triaxial measurement. Another common usage is to add unmeasured node locations that more completely describe a structural component (for example, corners of a panel where the test DOF were located interior to the edges).

The test display model must contain at minimum all the ASET nodes (test DOF) identified in step 3, though it can also contain additional nodes which will be useful in visualizing mode shapes. Any NASTRAN modeling/post processing tool can be used to generate a test display model, and IMAT can easily import the test display model and plot mode shapes. The nodes contained in the test display model are known as the display set.

 

Step 5 - Generate TAM Matrices using NASTRAN

Once you have identified the initial ASET and display set, you can now use NASTRAN to develop the TAM matrix and validate the selected ASET. Example files for this process are provided below:

Filename Description
plate_fem.blk Simple NASTRAN example for the following NASTRAN solution cases
plate_modes.dat

Modal solution of the plates model

plate_tam.dat

TAM solution

r1_aset.blk

First pass at the ASET DOF

r1_display.blk

First pass at the nodes in the display set

TDM.dat

Test display model (for visualization)

 

Step A: Create ASET and display set files

r1_aset.blk

r1_display.blk

The first step in developing the TAM matrix is to create the aset and display set files:

ASET file - This file can be generated by hand. See the NASTRAN Quick Reference Guide for the acceptable formats of ASET cards. You can also use the ctrace2aset IMAT command to create an ASET from a coordinate trace.

Display Set File - The display set is a comma separated list of the node numbers in the test display model. This set is used to specify the output nodes for nastran modal solution. In the TAM solution this set is used to control which nodes should be a part of the back expansion matrix.

Step B: Create the Modes Solve

plate_modes.dat

Creating the modes solve involves simply tweaking the standard modal solution used to identify the target modes.

INCLUDE 'r1_display.blk' - this command defines the output set 100 for the test display nodes

DISPLACEMENT(PUNCH) = 100 - This command specifies that the displacement output should be a punch file at the nodes defined by set 100 inside of the r1_display.blk file

Step C: Create the TAM Solution

plate_tam.dat

The TAM solution is a slightly more complicated modification of the modes run. Two modifications must be made to the standard modes solve:

1)The command EXTSEOUT(DMIGPCH,EXTID=200) should be inserted in the case control section of the deck. Note that the number given to the EXTID is not important, however the user should be careful that it does not overlap with the display set. This command is used to generate the back expansion matrix. Normally the command is used to output super elements, however it can also be used for the pretest process.

2) The r1_aset.blk file should be included in the bulk data section of the deck. This ensures that NASTRAN reduces the model to the selected test DOF.

 

Step 6 - Load TAM Matrices Using IMAT and Verify Pretest Analysis

Once PCH files from the modes and TAM solve have been generated with NASTRAN, the final step is to bring the files into IMAT and check to see if the selected ASET sufficiently represents the target modes. The first step is to use the load_tam function to import the punch files. This will generate the TAM, the TAM shapes - sa, and the analysis shapes - sg.

Next you will use the command report_tam_xml to generate an xml file, which can be opened using Microsoft Excel, to see the MAC and orthogonality values calculated based on the currently selected ASET DOF. A common goal is to require 0.95 or higher for the diagonal pseudo-orthogonality (POgg) terms of all target modes.

One common pitfall at this stage is outputting the results from your modes run and TAM run in different coordinate systems. This mismatch will result in poor MAC and Ortho matrices. Using the PCH files described in this tutorial helps to avoid this issue as all of the results are automatically output by NASTRAN in the local displacement coordinate system. Please note that the TAM shown in this example does an accurate job of capturing all 6 rigid body modes and the first 2 flexible modes of the structure.

The final step in this process is to use the TAM matrix to back expand the analysis shapes and see if there are any problems. This is checked both visually, by plotting the mode shapes before and after back expansion, as well as by using the orthogonality check.

In general it will take more than the first revision, r1_aset.bdf, to get you the orthogonality results you are looking for. The pretest procedure is iterative and it is a good idea to keep track of changes to the ASET by incrementing to r2_aset.bdf, r3_aset.bdf, and so on in order to keep track of how the ASET is evolving.

The above description can be executed using the following commands:

%% Load the TAM matrices

>> [tam sa sg] = load_tam('plate_tam.pch','plate_modes.pch');

%%

>> report_tam_xml(sg,sa,tam)

>> fem = readnas('TDM.dat')       % Read in the FEM from NASTRAN

>> fem = fem.fem                  % Extract the FEM from the NASTRAN input structure

%% Check back expansion matrix by back expanding FEM shapes

>> sg_bexp=backexp(sg,tam);

>> plot(sg_bexp,fem)

>> plot(sg,fem)