In Version 68 of MSC.Nastran, MSC introduced p-adaptive analysis using solid elements. The Patran MD Nastran Preference provides support for this new capability. There are some fundamental differences in approach to model building and results import for p-element analyses; this section will serve as a guide to these.

MSC.Nastran Version 69 extends the Version 68 capabilities for p-adaptive analysis in two areas. Shell and beam elements have been added and p-shells and p-beams can be used for linear dynamic solution sequences. Patran Version 6.0 supports both of these capabilities.

MD Nastran supports adaptive, p-element analyses with the 3D-solid CTETRA, CPENTA, and CHEXA elements; 2D-solid TRIA, and QUAD elements; shells TRIA, and QUAD elements; beams BAR elements. Patran and MD Nastran allow TET4, TET10, TET16, TET40, WEDGE6, WEDGE15, WEDGE52, HEX8, HEX20, and HEX64 for p-adaptive analysis for 3D-solids; tria3, tria6, tria7, tria9, tria13, quad4, quad8, quad9, quad12, and quad16 for p-adaptive analysis for 2d-solids and membranes; tria3, tria6, tria7, tria9, tria13, quad4, quad8, quad9, quad12, and quad16 for p-adaptive analysis for shells; bar2, bar3, and bar4 for p-adaptive analysis for beams. The preferred approach, when beginning a new model, is to use the higher-order elements--HEX64, WEDGE52, TET40, and TET16, or TRIA13 and QUAD16, or BAR4. The support for lower-order elements is provided primarily to support existing models. The higher-order cubic elements allow more accurate definition of the geometry and more accurate postprocessing of results from the MD Nastran analysis.The translator generates the appropriate MD Nastran FEEDGE and POINT entities for all curved edges on the p-elements. Models with HEX64 and WEDGE52 elements are easily created with the Patran Iso Mesher; models with TET16 elements can be created with the Tet Mesher. Models with QUAD16 and TRIA13 elements can be created using the Iso Mesher or the Paver.

For p-elements, Patran generates cubic edges to fit the underlying geometry. The cubic edge consists of two vertex grid points and two points in between. Adjacent cubic edges are not necessarily C1 continuous. If the original geometry is smooth, the cubic edges may introduce kinks which cause false stress concentrations. Then, the p-element produces unrealistic results especially for thin curved shells.

In Version 7 of Patran, for cubic elements, the two midside nodes on each edge are adjusted so that the edges of adjacent elements are C1 continuous. The adjustment is done in the Pat3Nas translator. After the Pat3Nas translator is executed, the location of the two midside nodes in the Patran database has changed. The user is informed with a warning message. The user can turn the adjustment of midside nodes ON and OFF with the environment variable PEDGE_MOVE. By default, the midside nodes are adjusted to make the adjacent elements C1 continuous. For PEDGE_MOVE set to OFF, the points on a cubic edge are not adjusted.

Patran generates the input for MD Nastran. For cubic edges, FEEDGE Bulk Data entries with POINTs are written. By default, the location of the two POINTs is moved to 1/3 and 2/3 of the edge in MD Nastran. The points generated by Patran must not be moved. Therefore, a parameter entry PARAM, PEDGEP, 1 is written by Patran. PEDGEP=1 indicates that incoming POINTs are not moved in MD Nastran. The default is PEDGEP= 0, MD Nastran will move the two POINTs to 1/3 and 2/3 of the edge. The C1 continuous cubic edges improve the accuracy of p-element results.

In the Version 69 Release Guide, a cylinder under internal pressure was tested to determine the quality of shell p-elements for curved geometry. The accuracy of the results was very good when exact geometry was used. With C1 continuous edges we recover the same quality of results within single precision accuracy.

Both element and p-formulation properties are defined using the Element Properties application by choosing Action: Create, Dimension: 1D/2D/ or 3D, Type: Beam/Shell/Bending Panel/2D Solid/Membrane/ or Solid, and p-Formulation on the main form. The details of the property form for this case are described on (p. 204). Most of the properties are optional and have defaults; the material property name is required.

Two properties that may need to be defined are Starting P-orders and Maximum P-orders. These properties specify the polynomial orders for the element interpolation functions in the three spatial directions. Although these are integer values, in Patran, each property is defined using the Patran vector definition. At first, this may seem peculiar, but it gives the user access to many useful tools in the Patran system for defining and manipulating these properties. Typically, a user would define these properties with a syntax like <3 4 2> to prescribe polynomial orders of 3, 4, and 2 in the X, Y, and Z directions. Patran will convert these values to floating point <3. 4. 2.>, but the Patran MD Nastran Preference will interpret them. This vector syntax is convenient primarily because it allows these properties to be defined using the Fields application. In a case where the material properties are constant over the model, but it is desirable to prescribe a distribution of p-orders, vector fields can be defined and specified in a single property definition. The Patran MD Nastran Preference will provide additional help for this modeling function. At the end of an adaptive analysis, when results are imported, vector, spatial fields will optionally be created containing the p-orders used for each element for each adaptive cycle. To repeat a single adaptive cycle, it is necessary only to modify the element properties by selecting the appropriate field.

A common use of the Maximum P-orders property is in dealing with elements in the vicinity of stress singularities. These singularities may be caused by the modeling of the geometry (e.g., sharp corners), boundary conditions (e.g., point constraints), or applied forces (e.g., point forces). Sometimes it is easier to tell the adaptive analysis to “ignore” these singular regions than it is to change the model. This can be done by setting the Maximum P-orders property for elements in this region to low values (e.g., <1 1 1> or <2 2 2>. These elements are sometimes called “sacrificial” elements.

It is well known in solid mechanics that point forces and constraints cause the stress field in the body to become infinite. In p-adaptive analyses, care must be taken in finite element creation and loads application to ensure that these artificial high-stress regions don’t dominate the analysis.

Generally, the best results are obtained with distributed loads (pressures) or distributed displacements. There are two options under Loads/BCs for applying distributed displacements. The Element Uniform and Element Variable types under Displacements allow displacement constraints to be applied to the faces of solid elements. If the elements are p-elements, the appropriate FEFACE and GMBC entries are produced. If applied to non-p-elements, the appropriate SPC1 or SPCD entries are produced.

Several new loads and boundary conditions support the p-shell and p-beam elements. Distributed loads can be applied to beam elements or to the edge of shell elements. Pressure loads can be applied to the faces of p-shell elements. Temperature loads can be applied to either the nodes or the elements.

Adaptive linear static and normal modes analyses are supported in Version 68 of MSC.Nastran; both solution types are supported by the Patran MD Nastran Preference. Only a few parameters on the Analysis forms may need to be changed for p-element analyses. If running a version of MSC.Nastran prior to Version 68.2 (i.e., Version 68, or 68.1), the OUTPUT2 Request option on the Translation Parameters form must be set to Alter File in order to process the results in Patran. The Solution Parameters forms for the linear static and normal modes analyses contain a Max p-Adaptive Cycles option, which is defaulted to 3. The Subcase Parameters form under Subcase Create has options to limit the participation of this subcase in the adaptive error analysis. Finally, the Advanced Output Requests form under Subcase Create has an option to define whether results are to be produced for all adaptive cycles or only every nth adaptive cycle.

Two different approaches are provided for postprocessing results from MD Nastran p-element analyses. Both approaches rely on MD Nastran creating results for a “VU mesh” where each p-element is automatically subdivided into a number of smaller elements. In the standard approach with the default MD Nastran VU mesh (3 x 3 x 3 elements) for solids, (3 x 3 elements) for shells and (3 elements) for beams, the results will automatically be mapped onto the Patran nodes and elements during import. This mapping will occur for all 10, Patran solid element topologies mentioned above. The most accurate mapping and postprocessing takes place when results are mapped to the higher-order Patran elements.

When the adaptive analysis process increases the p-orders in one or more elements beyond 3, the 3 x 3 x 3 VU mesh, mapping, and postprocessing may not be sufficiently accurate. The Patran MD Nastran Preference provides a second approach to handle this situation. In this case, a user can specify a higher-order VU mesh (e.g. 5 x 5 x 5) on the MD Nastran OUTRCV entry and then import both model data and results entities into a new, empty Patran database. In this case, the VU mesh and results are imported directly, rather than mapped and can be post-processed with greater accuracy. The OUTRCV entry is currently supported only with the Bulk Data Include File option on the Translation Parameters form.

It should be noted that, with this import mode, displays of element results (e.g., fringe plots) may be discontinuous across parent, p-element boundaries. This occurs because the VU grids generated by MD Nastran are different in each p-element. Along element boundaries there are coincident nodes and a result associated with each one. The user should not try to perform an Equivalence operation to remove these coincident nodes. If this is done, subsequent postprocessing operations will likely be incorrect.

For both postprocessing options, a result case is created for each adaptive cycle in the analysis. The result types in this result case will depend on specific options selected on the Output Request form. By default, the Adaptive Cycle Output Interval option is equal to zero. This means that output quantities specific to p-elements will be written only for the last cycle. If postprocessing of results from intermediate cycles is desired, the Adaptive Cycle Output Interval option should be set equal to one.

One of the key uses of output from intermediate adaptive cycles is in examining the convergence of selected quantities (e.g., stresses). This can be done using the X-Y plotting capability under the Results application.

There are several areas where a user can encounter problems producing correct p-element models for MD Nastran. One is the incorrect usage of the midside nodes in the Patran higher order-elements. These nodes are used in p-element analysis only for defining the element geometry; analysis degrees of freedom are not associated with these nodes. Therefore it is illegal, for example, to attach non p-elements to assign loads or boundary conditions to these nodes. One way this can occur inadvertently is if a nodal force is applied to the face of a Patran solid. This force is interpreted as a point force at every node (including the midside nodes) on the face of the solid. For the p-elements, this is not valid. This type of load should instead be applied as an element uniform or element variable pressure.

Modifying an existing solid model for adaptive, p-element analysis is relatively straightforward. The first step is to read the NASTRAN input file into Patran using the Analysis/Read Input File option. The model may contain any combination of linear or quadratic tetra, penta, or hexa elements. The second step is to use the Element Props/Modify function to change the Option for all solid properties from Standard Formulation to P-Formulation. The element properties form for p-formulation solids has many options specific to p-element analysis; but they all have appropriate defaults. This property modification step is the only change that must be made before submitting the model for analysis.

Often, however, as discussed in Potential Pitfalls, 21, it is appropriate to modify the types of loads and boundary conditions applied to the model. For example, in non p-element models, displacement constraints are applied using MD Nastran SPC entries at grid points. In p-element analyses, element-oriented displacement constraints are more appropriate. Existing displacement LBCs can be modified using the Loads/BCs/Modify/Displacement option. For an SPC type of displacement constraint, the LBC type is nodal. For a p-element analysis, Element Uniform or Element Variable displacement constraints are more appropriate. The application region must be changed from a selection of nodes to a selection of element faces. As described above, nodal forces can be troublesome in p-element analyses. If possible, it is beneficial to redefine point forces as pressures acting on an element face. If this is not possible, an alternative is to limit the p-orders in the elements connected to the node with the point force; this can be done by defining a new element property for these elements and defining the Maximum P-orders vector appropriately. Element pressures, inertial loads, and nodal temperatures defined in the original model need not be changed for the p-element analysis.