The Bulk data section is composed of entries; each entry contains data distributed in fields. Each line has has 10 fields. The entry name is given in the first field of the first line. The tenth field in each line serves to indicate whether there is an additional line in the entry. An example of this structure can be seen in Figure 2.

Figure 2: Example of an entry in the Bulk data section.

Data can only be integer, real o string. A string has at most 8 characters. Reals can be written in several ways; for example, 7.0, .7E1, 0.7+1, .70+1, 7.E+0 y 70.-1 are the same number.

MD Nastran has three different formats for data in an entry:

• Free Field Format: data fields are separated by commas;
• Small Field Format: there are 10 contiguous fields, each of them is 8 characters long;
• Large Field Format: there are 10 contiguous fields, each of them is 16 characters long.

The FE types are defined as entries in the Bulk data section, described in Chapter 8 of the MD Nastran 2006 Quick Reference Guide. The name of the entries supported by feconv are CTRIA3, CTRIA6, CQUAD4, CQUAD8, CTETRA, CPENTA and CHEXA. Only CTRIA3 and CTETRA has been tested. In Figure 3 and Figure 4 we show the definition of such entries.

Figure 3: Definition of entry CTRIA3.

Figure 4: Definition of entry CTETRA.

Those entries store the connectivity of the mesh, that is, the content of variables mm and nn of the MFM format.

For CTRIA3 and CTETRA entries, if the determinant of the matriz of the transformation to the reference element is negative, the last two vertices are exchanged to get a positive determinant.

The node coordinates are defined in the Bulk data section, in the entry named GRID. That gives us the variable z of the MFM format. In Figure 5 we show the definition of such entry.

Figure 5: Definition of entry GRID.

The domain references are useful to assign physical properties to subdomains. This information is collected from the PID field of the aforementioned entries. That gives us the variable nsd of the MFM format.

References are useful to apply boundary conditions to the mesh. We distiguish between natural boundary conditions, also called Neumann conditions, and the essential boundary conditions, also called Dirichlet conditions. Dirichlet conditions are imposed as Displacement in MD Nastran and Neumann conditions are imposed as Force. Where both conditions are applied, Dirichlet prevails over Neumann.

Boundary conditions can be imposed on nodes, edges or faces. In the MFM format, those conditions are stored in variables nrv, nra and nrc, respectively. While it is easy to transform face and edge references to node ones, there can be problems doing the inverse conversion; these difficulties are described in section Converting node references to edge and face references.

Dirichlet conditions applied to nodes are read in feconv from entries SPC and SPC1 in the Bulk data section. The definition of the entry SPC can be seen in Figure 6.

Figure 6: Definition of entry SPC.

Detection of entry SPC was included in feconv because is the default entry used in Hypermesh to set Dirichlet conditions applied to nodes. There are several issues associated with this entry that we describe below:

• In order to know how many different conditions are present in the mesh, we cannot use the field SID since, as far as we know, Hypermesh always assigns it value 1; we consider instead the value of every displacement, written in the Di field, to group nodes by references.
• 6 different restriction degrees can be applied to every node (3 displacements and 3 rotations); every degree is identified in the Ci field with a number from 1 to 6.
• Restrictions for the same node can be saved in different SPC entries. To manage them Hypermesh follows two rules:
• all the SPC entries for the same condition are contiguous, and
• for the same condition, degrees are set in ascending order; for example, if fixed, degree 1 is set before degree 2.
• feconv uses the previous rules to deal with SPC entries. As an example, consider one SPC entry that restrict degrees 1 and 2, and assign them value 8, another one that restrict degrees 3 and 4 with value 10 and a third one for degree 2 with value 7; therefore, we have two reference conditions, the first one restricts degrees 1, 2, 3 and 4 with values 8, 8, 10, 10, respectively; the second one only restricts degree 2 with value 7.
• We only know the total number of conditions after all have been read; thus, we use procedure set_SPC of module module_desplazamientos to store all the conditions due to SPC entries for each node; then, we call procedure assign_SPC to group nodes that belong to the same condition.
• In feconv, when two conditions are assigned to the same node, the one with the biggest reference number will be assigned.

A FORCE entry manages Neumann conditions. The module module_fuerzas deal with these entries in feconv.

Different Neumann conditions are set attending to the value assigned in the Ni field; the SID field is not considered. The definition of the entry FORCE can be seen in Figure 7.

Figure 7: Definition of entry FORCE.

As it was explained for the SPC field, procedure set_FORCE saves all the conditions and procedure assign_FORCE asigns to node the condition with the biggest reference number, provided there is no Dirichlet condition applied to it.

Converting node references to edge and face references

Many solvers require boundary conditions assigned to edges and faces. To do so, we have implemented in feconv two methods:

• to transform the node conditions read in SPC, SPC1 and FORCE entries into edge and face conditions;
• to interpret finite elements of smaller dimension as edge and face conditions.

Transforming node references

The transformation of node references to edge references is done in procedure dos; to face references is done in procedures tres and cuatro.

The rules for the transformation are:

• if all the vertices of the entity (edge or face) have the same reference, this one is also applied to the entity;
• if some vertex has no reference assigned (i.e. has reference 0) then no reference is assigned to the entity;
• if the vertices have references of different type, the Neumann condition with the lowest reference number is assigned to the entity;
• otherwise, the reference with the lowest reference number is assigned to the entity.

These rules guarantee that the edges or faces that are in the border between two conditions have assigned Dirichlet over Neumann condition and also the biggest reference number.

You must aware that this rules can fail in some corners. Figure Figure 8 shows a border, as a bold line, between reference conditions 1 and 2. In the finite element of the corner, every vertex has reference 2, making unavoidable that the reference assigned to its edges (and face) will be also 2.

Figure 8: Asignment rules can fail in a corner.

In order to avoid such drawback, we have implemented an alternative way to apply edge and face conditions.

Interpreting FE of smaller dimension

The transformation we will describe here is preferred over the explaind in the previous section, since it does not present the aforementioned drawback. Both types of transformation are applied, but the present one has priority over the first transformation, because it is set after it.

Since the MFM format does not allow hybrid meshes, and this format is the "lingua franca" of feconv, all the finite elements of smaller dimension present in the input file are generally discarded. We have use them to indentify references.

In meshes composed of finite elements defined in CTRIA3 or CTRIA6 entries, every CBEAM entry is interpreted as an edge reference condition; the number associated to that reference is the value stored in the PID field.

In meshes composed of finite elements defined in CTETRA entries, every CTRIA3 entry is interpreted as a face condition; the number associated to that reference is the value stored in the PID field.