MSC Nastran, Solution 101, Linear Statics, CBAR Bar Elements with Standard Formulation

Upon substitution of the engineering data into the equations below, the following results are obtained:

To determine the deflections at the free end of the frame, the model shown in Figure 14‑1 was created. This model consisted of 14 MSC Nastran CBAR elements. Each bar was assumed to have a square cross-section of 0.5 x 0.5 inches. This gives a cross-sectional moment of inertia of 0.0052083 in4 that is identical to what was assumed in the preceding calculations. Using this model, the following results were obtained.

*MSC Nastran results have opposite sign due to the reversal of the direction of x and z axes of the global coordinate frame relative to the theoretical results coordinates.

The corresponding deformed shape plot that was made for the rigid frame is shown in Figure 14‑2 where the deformed shape has been superimposed upon the undeformed mesh. Fringe plots for the x, y, and z components of the translational displacements that were generated with Patran are shown in Figure 14‑3, Figure 14‑4 and Figure 14‑5, respectively. The fringe plot for the rotation about the z axis is shown plotted in Figure 14‑6. All fringe plots are displayed on the fully deformed structure. Examination of these fringe plots near the free end of the frame clearly shows that the Patran results are identical to the preceding MSC Nastran results.

MSC Nastran, Linear Statics, Solution 101, CQUAD4 Elements with Standard Formulation and Laminated Material Properties.

To predict the stresses in the cross-ply laminate for this problem, a model was created that consisted of CQUAD4 elements with laminate properties specified by a MSC Nastran PCOMP data entry. This permitted stress recovery to be performed on a ply by ply basis. Due to symmetry, any motion along the vertical and horizontal planes of symmetry was restrained out. In addition, all out of plane deformations were restrained since a balanced cross-ply laminate should remain flat during cool down. Application of these boundary conditions avoided any potential problems with unrestrained rigid body motion. The applied loads and boundary conditions are also shown superimposed upon the finite element mesh in Figure 14‑7.

Using this model, the following results were obtained with MSC Nastran.

The corresponding fringe plots that were generated with Patran for the x-, y- and xy shear stress components in each of the plies are shown in Figure 14‑8 through Figure 14‑16. A comparison of these plots with the preceding MSC Nastran results clearly shows that the two are identical. Layer 1 and 3 were plotted in the element coordinate system; layer 2 was plotted in the Global coordinate system. You must read in the .bdf file below to be able to perform the correct coordinate transformation to reproduce the layer 2 plots.

MSC Nastran, Solution 101, Linear Statics, CQUAD4 Elements with Standard Formulation.

Transverse Shear Force:

 

where  

 

Moments:

Fiber and Shear Stresses:

Stress at a:

Stress at b:

Stress at c:

Stress at b’:

Stress at a’:

To determine the stress state in the beam, a MSC Nastran model was generated using Patran. To maximize accuracy, a mesh density was chosen so that nodes would be precisely situated at every designated stress recovery point. In addition, to prevent any out of plane deformation, all displacements normal to the plane of the model were fully restrained, thereby imposing a plane strain condition. Furthermore, to prevent any longitudinal rigid body translation, a symmetry boundary condition was imposed at midspan the entire height of the beam. The imposed boundary conditions and applied loads are shown in Figure 14‑17 superimposed upon the mesh, which consisted solely of CQUAD4 elements using a standard formulation. Using this model, the following stresses were predicted at points a, b, c, b’ and a’.

The Patran fringe plots that were made of the x-, y- and xy- stress components are shown in Figure 14‑18, Figure 14‑19, and Figure 14‑20 respectively. In addition, the orientation angle for the max principal stress, or zero shear angle, has been plotted in Figure 14‑21. To better show the stress state at each of the designated stress recovery points, tensor plots were made of the fiber stress as well as the principal stress at each position, starting with a and proceeding onto a’. These are shown in Figure 14‑22 through Figure 14‑26. Examination of the Patran tensor and fringe plots reveals that they are identical to the preceding MSC Nastran results.

MSC Nastran, Linear Statics, Solution 101, CQUAD4, CQUAD8, CTRIA3, CTRIA6, CQUADR and CTRIAR Elements with Standard and Revised Formulations

For the purposes of this problem, a 15 degree segment was modeled of the cross-section of the pipe with the appropriate axisymmetric boundary conditions being applied to the lateral edges of the model. In addition, five individual segments were modeled that were meshed with either CQUAD4, CQUAD8, CTRIA3 or CTRIA6 elements using a standard formulation or CQUADR and CTRIAR elements with a revised formulation. This was done to assess how variations in element topology and formulation affect overall accuracy of the results when performing a plane strain analysis with a high Poisson’s ratio. The actual model that was generated with Patran is shown in Figure 14‑27 where the individual element types associated with each segment have been identified. The loading and boundary conditions that were applied to the model are shown in Figure 14‑28.

* Represents average of all edge nodal values with nodal values averaged across adjacent elements.

The fringe plot that was generated for the radial displacement is shown in Figure 14‑29. Fringe plots for the radial and hoop stress are shown in Figure 14‑30 and Figure 14‑31. Here the stresses have been plotted with an adjusted scale that better shows the stress gradient present in each of the segments. All plots have been transformed into the cylindrical coordinate system defined in the problem. A comparison with the preceding tabular results clearly shows that Patran is accurately reproducing the MSC Nastran results.

The preceding results clearly demonstrate the wide degree of variability in the result attributable to element topology as well as formulation. Consistently, the higher order CQUAD8 and CTRIA6 elements gave superior performance compared to their linear counterparts. Similarly, in this application where cylindrical geometry was involved, a triangular element gave far more accurate results then compared to a quadrilateral element. Only by adopting the revised formulation of a CQUADR could acceptable results be obtained with a quadrilateral element. This would not be unexpected since the removal of any membrane-bending coupling produces far less sensitivity to extreme values in Poisson’s ratio as in this example.

MSC Nastran, Linear Statics, Solution 101, CQUAD4 and CTRIA3 with Standard Formulation

For the case of an internally pressurized spherical shell tangentially supported, the predicted stresses and displacements are, after substituting the assumed values for :

A model of the spherical shell was created using Patran. Due to symmetry, only one fourth of the shell was modeled with the appropriate axisymmetric boundary conditions applied to the free edges. The model that was created is shown in Figure 14‑32. The majority of the model was meshed with CQUAD4 elements, with the mesh becoming increasingly refined near the center of the shell. Only at the very apex of the shell are CTRIA3 elements used. However, every attempt was made to minimize having high aspect ratio triangular elements that would otherwise cause a loss of accuracy. Using this model, the following results were obtained.

The corresponding fringe plots for the radial displacement and the x-displacement in global coordinates are shown in Figure 14‑33 and Figure 14‑34. The radial displacement plot gives whereas the max value shown on the x-displacement plot corresponds to . In Figure 14‑35, the y-displacement in global coordinates is plotted. The difference between the maximum and minimum y-displacements corresponds to above, or the change in vertical height for the shell. Fringe plots for the radial, meridional and circumferential stresses are shown in Figure 14‑36 through Figure 14‑38. A comparison of the Patran fringe plots with the MSC Nastran results shows an exact correlation between the two.

MSC Nastran, Linear Statics, Solution 101, CTRIAX6 Elements, 2D Axisymmetric Solids

Two models were created with Patran of the thick walled cylinder. One featured 3 noded and the other 6 noded CTRIAX6 elements. Both models used the same number of elements. The models with the applied loading are shown in Figure 14‑39, which was assumed to be a uniform external ambient pressure of 1000.0 psi. Using these models, results were obtained and the following errors occurred relative to the theoretical values for each of the element topologies that were examined. The results clearly show the expected behavior; namely, the presence of the end caps reduces the inward radial contraction at the center of the cylinder. This necessarily reduces the predicted hoop stress relative to the theoretical value. The only stress components that should correlate with the theoretical values are the radial stress at the ID and OD of the cylinder ad the axial stress at the mean radius of the cylinder.

The fringe plots created of the radial displacement are shown in Figure 14‑40 and Figure 14‑41. The range has been adjusted to better show the displacement at the center of the cylinder. Similarly, the radial stress distribution is shown in Figure 14‑42 and Figure 14‑43; the hoop stress in Figure 14‑44 and Figure 14‑45; and the axial stress in Figure 14‑46 and Figure 14‑47. A comparison of the Patran fringe plots with the preceding tabular results clearly reveals that the MSC Nastran results are being accurately displayed.

MSC Nastran, Linear Statics, Solution 101, CHEX8 Elements - 3D Solids

This is a repeat of Problem 6: Linear Statics, 2D Axisymmetric Solids, 42 with the exception that the cylinder and end caps are entirely modeled with MSC Nastran 3D solid HEX8 elements. In addition, all analytical results are recovered in a global cylindrical coordinate frame. This should produce results that are identical to those recovered with CTRIAX6 2D axisymmetric solid elements.

A model was created of the thick walled cylinder with the end caps using just MSC Nastran 3D solid CHEX8 elements. Due to symmetry, only one eighth of the cylinder was modeled, with the appropriate axisymmetric and symmetry boundary conditions applied to the free faces of the model. The model that was created is shown in Figure 14‑48 and the applied boundary conditions in Figure 14‑49. Using this model, the results below were computed at the middle of the cylinder.

MSC Nastran, Linear Statics, Solution 101, CROD 1D Elements.

The theoretical solution was calculated by using the matrix equation on page 159 of the reference using the values listed above for . The results are as follows:

Displacements:

Element Forces:

Due to the pinned construction of the truss, all members are only capable of carrying axial loads. This necessitated that the truss be modeled using MSC Nastran 1D CROD elements. The model that was created using Patran is shown in Figure 14‑55. Note that each truss member was modeled using a single CROD element. The loads and boundary conditions that were applied to the model are also shown in Figure 14‑55.

The following results were obtained with MSC Nastran.

The corresponding color fringe plots that were made in Patran of the x- and y-components of displacement are shown in Figure 14‑56 and Figure 14‑57, respectively. For the purposes of these plots, the target entity was set to nodes and the averaging domain was specified as all entities. The rod forces and stresses that were predicted by MSC Nastran are shown in Figure 14‑58 and Figure 14‑59, respectively. Unlike displacements, it was necessary to set the target entity to elements and the averaging domain to individual. This avoided having any averaging across adjacent elements which otherwise would have given an inaccurate representation of the actual results. A closer inspection of these plots reveals that the results that are being shown are in fact identical to those predicted by MSC Nastran.

MSC Nastran, Nonlinear Statics, Solution 106, Shell Element with Standard Formulation, CQUAD4 and CQUAD8

Timoshenko, S., and Woinowsky-Krieger, S., Theory of Plates and Shells, McGraw-Hill, Inc., 1959, p. 422.

A square plate with clamped edges is loaded uniformly such that the center deflection exceeds the plate thickness. Considering large deflection effects (small strain theory), find the deflection at the center of the plate.

The following diagram summarizes the theoretical solution for the case when large deflection effects are both considered and ignored.

For , with nonlinear effects.

For , without nonlinear effects.

Due to symmetry, only one-fourth of the plate was modeled. The outer edges were fully restrained while the appropriate symmetry boundary conditions were imposed along the remaining free edges and at the center of the plate. Two models were created. The first was meshed with MSC Nastran CQUAD4 elements which have a finite strain formulation needed to incorporate large deflection effects. The second model was meshed with CQUAD8 elements, which do not have a finite strain formulation. Both models along with the applied loading and imposed boundary conditions are shown in Figure 14‑60 and Figure 14‑61. The MSC Nastran results that were obtained are summarized below and plotted in Figure 14‑62 and Figure 14‑63.

It should be noted that although both analyses were conducted using MSC Nastran, Solution 106 with large deflection effects included, the analysis performed with CQUAD8 excluded any geometric nonlinearities since this type of element has no finite strain formulation. This illustrates the care that must be exercised when performing a nonlinear statics analysis with mixed element types. The same problem exists for CTRIA3 and CTRIA6 elements.

MSC Nastran, Linear Statics, Solution 101, Solid Elements With Standard Formulation, CHEXA (8 and 20 noded), CPENTA (6 and 15 noded), CTETRA (4 and 10 noded).

To demonstrate that thermal stress effects can be properly recovered for all of the various solid element topologies supported by MSC Nastran, a simple model was created that consisted of 6 cubes. Each cube was subjected to three independent linear temperature gradients of 100, 200 and 300 degrees F per inch along the x, y and z axes, respectively. The cubes were meshed with either HEX8, HEX20, WEDGE6, WEDGE15 TET4 or TET10 elements with a mesh density of one element per edge. The model that was created is shown in Figure 14‑64 and the applied temperatures are shown in Figure 14‑65.

The maximum von Mises stress that was computed by MSC Nastran for a given element topology are summarized below.

The corresponding deformed shapes and von Mises stress contours that were generated using Patran are shown in Figure 14‑66 and Figure 14‑67, clearly showing the high residual stresses that were generated in both the degenerate WEDGE6 and TET4 elements. The peak values for the von Mises stress shown are somewhat less than those shown in due to the nodal averaging of results at adjacent elements.

Ideally, the presence of a weak elastic support should have provided minimal restraint to thermal expansion, resulting in a near zero stress state. This behavior was observed in both the HEX8 and HEX20 elements as well as the higher order TET10 and WEDGE15 elements. The extremely high stresses observed with TET4 and WEDGE6 elements would not be unexpected since these elements tend to be excessively stiff resulting in a loss of accuracy. Consequently, the results illustrate the care that must be exercised when modeling with the solids and the need to avoid excessive use of degenerate elements, especially in areas where high stress gradients are predicted to occur, such as at the vertices of the cubes in this particular problem.

MSC Nastran, Linear Statics, Solution 101, Simple Shell Elements, CQUAD4 and CTRIA3

The resultant deformation for a simply supported annular plate can be derived by summing the deformations obtained for a flat circular plate subjected to the same pressure load, an annular plate carrying along its inner edge a shear force per unit circumferential length of and an annular plate with a distributed radial bending moment of . All of the plates have the same outer radius and the both annular plates have the same inner radius.

According to reference (2), the maximum deflection occurs at the inner radius and is given by the expression:

body

For the purposes of this problem, models of a flat circular and annular plates where created in Patran using the following dimensions, applied loading and material properties:

The model that was generated for a uniformly pressurized circular plate is shown in Figure 14‑68. Due to symmetry, only a 90 degree sector of the plate was modeled with axisymmetric boundary conditions being applied along the lateral edges of the sector. The center of the plate was constrained to move only in the vertical direction. Between the inner and outer radius of the annular plate, a mesh consisting of CQUAD4 elements was used to maximize accuracy. Conversely, inboard of the inner radius, a CTRIA3 mesh was used to avoid having badly distorted CQUAD4 elements that might otherwise result in a loss of accuracy. By having the mesh transition coincide exactly with the edges of the annular plate, this permitted using a single model to investigate the behavior of a complete circular plate as well as an annular plate, with the elements corresponding to just the annular and the complete plate being assigned to a different groups within Patran. The corresponding models that were used to investigate the case of an annular plate subjected to either a distributed edge shear or moment are shown in Figure 14‑69 and Figure 14‑70.

Substitution of the model parameters into equations (14‑1) through (14‑6) yields a maximum deflection at the inner radius of

The value derived within Patran was -.8799 in, or a deviation of approximately 0.69% from the theoretical value

MSC Nastran, Nonlinear Statics, Solution 106, CBEAM, 1D Beams with Standard Formulation.

The post-buckled beam end coordinates and critical buckling load are given by the equations below. The integrals and are known as the complex elliptical integral of the first and second kind, respectively. Their values are typically listed as a function of sin-1(p). For a known deflection angle of =600, the required the load and tip deflection can be derived as shown here

To determine the post-buckled shape for the beam, the model shown in Figure 14‑83 was generated using Patran. The model consisted of 20 1D CBEAM elements that used a standard generalized formulation. To ensure that the beam will deflect laterally, a slight horizontal load was applied to the beam in addition to an axial load of 2984.73 lbs. In this case a lateral load of 10 lbs was used. In addition, since the structure is post-buckled, it is inherently unstable. This requires that the user set the MSC Nastran parameter TESTNEG to -2 in the input file.

The following results were obtained with MSC Nastran.

The corresponding Patran fringe plots that were made of the horizontal and vertical displacements are shown in Figure 14‑84 through Figure 14‑85. Deflection plots were set to True Scale as opposed to a percentage of the model. The rotation about the global z-axis given in radians is shown in Figure 14‑86. For the purposes of evaluating the accuracy of these plots, it is necessary to use the following conversions:

where and are the MSC Nastran horizontal and vertical nodal displacements, respectively. Vector plots of the translational and rotational displacements are shown in Figure 14‑87 and Figure 14‑88. After making the appropriate conversions, it is apparent that the Patran results are identical to those obtained with MSC Nastran.