Example 1 – Manual inertia relief INREL,-1 – GRDPNT,1

The following example is taken form the NX NASTRAN User’s Guide (Ref. 1).  This simple example shows the method, as well as the effects, of using different SUPORT points when using manual inertia relief, as well as using automatic inertia relief.

A three CBEAM structure is to be analyzed as a free-free structure with a line load acting in the Y-direction, shown in Figure 1.  To show the effect of the SUPORT point, two manual inertia relief runs are made, each with a different SUPORT grid point.  In addition to these manual inertia relief runs, an automatic inertia relief analysis will be performed on the same model.

Figure 1: Three-CBEAM model used in the inertia relief example (image via ref. 1)

In an attempt to better describe the physics of the inertia relief theory, selected hand calculations are performed and compared to the NASTRAN result files.  The selected calculations include the resultant of the applied loads about the GRDPNT, as well as a calculation of the load necessary to impose unit acceleration about the SUPORT point.

Example 1 – Manual inertia relief INREL,-1 – GRDPNT,1

The first section in this example involves using manual inertial relief with both the SUPORT and GRDPNT defined at node 1.  The SUPORT (reference) degrees of freedom are specified in the format shown in Figure 2.

Figure 2: SUPORT entry format (image via ref. 1)

All 6 degrees of freedom are defined in the SUPORT entry at node 1.  The input deck for this analysis is shown in Figure 3.  This input deck contains the SUPORT and GRDPNT entries for all three analyses with those for the second and third analyses (manual w/ SUPORT and GRDPNT at node 3 and automatic inertia relief) commented out.

Figure 3: Input deck for Example 1 three-CBEAM model analysis with inertia relief

Hand calculations for the resultant of applied loads about GRDPNT as well as the load necessary to impose unit acceleration in the Y-direction are shown in Figure 4.  Results from these calculations can be compared to the results from NASTRAN, shown in Figure 5.

Figure 4: Hand calculations for Example 1

A portion of the NASTRAN output file (.f06 file) for this analysis is shown in Figure 5.  The Grid Point Weight Generator (GPWG) is calculated with respect to the grid point specified in the GRDPNT entry.  Model mass, 0.2229 lbf for this example, and inertia can be verified here.

Following the GPWG is the OLOAD resultant, which contains seven sections with seven lines each.  The first section describes the resultant of the applied loads about the GRDPNT.  The following six sections describe the loans necessary to impose unit acceleration about the SUPORT point.  Sections 2-7 correspond to directions X, Y, Z, RX, RY, RZ, respectively.  Results from the hand calculations can be compared to those found in the OLOAD table.  OLOAD results corresponding to the hand calculations shown in Figure 4 are circled in blue.

Following the OLOAD table in the output file is the User Information Message 3035.  This message displays the strain energy and epsilon that results from the unit acceleration imposed about the SUPORT point.  These strain energy and epsilon values should always be checked to verify that they are very small, ensuring that there are not any unwanted constraints in the model.  Strain energy and epsilon values are circled in red in the NASTRAN output file shown in Figure 5.

Following UIM 3035 in the output file are the QRR, QRL, and URA matrices.  The QRR matrix (6×6) is the total rigid body mass of the structure taken about the GRDPNT.  Next is the QRL matrix describing the resultant of the ‘apparent reaction loads” measured about the SUPORT point.  This result should be equal and opposite to the values in the first section of the OLOAD table.  The final matrix is the URA matrix describing the rigid body acceleration computed from the applied loads.  These three matrices should follow the general F=ma formula (i.e. [QRL] = [QRR][URA]).

Toward the end of the output file are the displacement and stress outputs.  Notice that the displacement at the SUPORT point (node 1 for this example) is 0.  All of the remaining displacements in the model are relative to this SUPORT point.  SPC forces are shown to confirm that the loads are balances at the SUPORT point.

Figure 5: NASTRAN results file for Example 1