4.5 Solids

In RFEM, 3D objects are described by solids. When generating the FE mesh, 3D elements are created. You can also use solids to model orthotropic properties or contact problems between surfaces. In addition, solids can have gas properties.

In general, boundary surfaces of solids are defined with the stiffness type Null (see Chapter 4.4). However, if no other solid is connected to a model that represents the contact between two surfaces, both contact surfaces have to be characterized with a stiffness.

In the list of the dialog box and the table, several stiffness types to realistically model structures can be selected. Each type has its own color that can be used to differentiate solids in the model. Colors are controlled in the Display navigator using the Colors in Rendering According to option (see Chapter 11.1.9).

The standard model is represented by a 3D object with the solid-specific properties of a homogeneous and isotropic material. Therefore, boundary surfaces should be defined by the stiffness type Null.

If the solid has orthotropic properties, stiffnesses are also derived from the material characteristics. Define the elastic stiffnesses of the three-dimensional material model in the Material Model - Orthotropic Elastic 3D dialog box (see Figure 4.49).

Use this option to model solids with properties of an ideal gas (e.g. tank, bouncy castle, insulating glass). The gas parameters have to be defined in a separate tab of the dialog box (see Figure 4.84).

The solid type Contact is suitable for modeling contact properties between two surfaces. The parameters have to be defined in a separate tab of the dialog box (see Figure 4.83).

Neither a null solid nor its loads are considered for the calculation. Null solids are, for example, used to analyze changes in the model's structural behavior if a solid is not effective. You do not need to delete the solid, the loading is kept as well.

A solid is defined by surfaces that completely enclose a certain space. Enter the numbers of the surfaces into the text box or select them in the graphic using the button.

When you have defined all boundary surfaces in the New Solid dialog box, use the [Show Figure or Rendering] button below the graphic to see a preview of the solid.

You can select an entry from the list of materials that have already been created. Material colors make the assignment easier.

In the New Solid dialog box, you can see three buttons below the list. Use the buttons to access the material library or to create and edit materials.

For more detailed information about materials, see Chapter 4.3.

When an intersection of solids has been created, this column is displayed in the table.

In addition to surfaces, you can generate intersections for solids. RFEM determines the intersection lines of intersecting solids and creates 3D solid objects as a union, a section, or as a pure intersecting set. In this way, a new solid is generated from the two original objects.

You can create intersections of solids quickly in the graphic: Select two solids by drawing a selection window across the objects or using a multiple selection by holding down the [Ctrl] key. Then, right-click one of the solids to open its shortcut menu where you select the menu item Solid → New Compound Solid.

The New Solid dialog box opens. With the settings in the Compound Solids dialog tab, you can specify how both solids are combined.

The numbers of the two selected solids have already been entered into the text boxes. Use the list or to change the entries.

There are three ways to combine solids into a new object:

• Unite: Solids A and B are merged into a unit.

• Subtract: Solid B is cut out of solid A.

• Intersect: RFEM determines the area shared by solids A and B.

The dialog graphic to the right demonstrates the principle of the individual combinations. Use the [Show Figure or Rendering] button to switch between scheme and model display.

The Option dialog section allows you to control how parts that were cut are displayed in the graphic of the work window. When subtracting solids, you can use the as hole option to model boreholes, for example.

Click [OK] to create the combined solid. As a result, intersections of surfaces (see Chapter 4.22) with active or inactive surface components (see Chapter 4.4) are generated. At the same time, RFEM sets the original solids to the type Null.

This table column shows the volume of each solid.

The mass of each solid is indicated in the penultimate column. It is determined from the volume and the material's specific weight.

This dialog tab is available if you have selected the solid type Gas in the General dialog tab.

In this tab, you have to define the Gas Parameters pressure p_p and temperature T_p.

This dialog tab is available if the Contact solid type has been selected in the General dialog tab.

• Both contact surfaces must be arranged to be parallel and created identically. It is recommended to create the second contact surface by copying the first one.
• Each lateral connecting surface between the contact surfaces must be created as a simple surface consisting of four boundary lines. Splitting a connecting surface into two surface components at half of the height, for example, is not allowed.
• When modeling curved contact surfaces, you have to split the contact solid into several simple parts.
• RFEM generates undivided 3D elements (parallel "columns") between the finite elements of the contact surfaces, creating a direct connection. Therefore, the FE division of the surface needs to be adjusted to the spacing of the contact surfaces.
• Polygonal solids are preferable to triangular solids.

RFEM tries to find the contact surfaces automatically. In the Contact Between Two Surfaces dialog section, you can change Surface A by using the list or use to select it graphically. RFEM automatically enters Surface B as the solid surface that is parallel to the first surface.

In the Contact Perpendicular to Surfaces dialog section, you can select between three options:

• Full force transmission
• Failure under compression
• Failure under tension

The failure criteria Failure under compression and Failure under tension are taken into account in the calculation via the deformations of solid FE mesh nodes.

The Contact Parallel to Surfaces can be defined independently of the contact properties that act perpendicular to the two contact surfaces.

The contact criteria parallel to surfaces are defined as follows:

Table 4.2 Contact properties parallel to contact surfaces

Contact	Diagram	Description
Failure if contact perpendicular to surfaces failed		If the contact solid under tension or compressions fails, no shear forces are transmitted.
Full force transmission		All shear forces are transmitted.
Rigid friction		The rigid friction is immediately effective. The shear stress is dependent on the normal stress. You have to enter the friction factor μ.
Rigid friction with limit		As soon as the maximum permitted shear stress τmax is reached, the stress is not increased any further by extending the deformation, but remains constant.
Elastic friction		This friction represents an elastic behavior: The shear force increases proportionally to the deformation. There is no limit for deformation. The spring stiffness C (the force required to move a 1 m2 surface by 1 m) and the friction factor μ must be entered as parameters.
Elastic friction with limit		Unlike with the elastic friction, the maximum shear stress does not depend on the normal stress: Only one defined shear stress can be absorbed. The spring stiffness C and the shear stress τmax must be entered as parameters.
Elastic solid behavior		The properties of the elastic shear transfer can be described by entering the spring stiffness C.

The FE Mesh dialog tab allows you to set specific requirements for each solid concerning the FE mesh.

To allocate an FE Mesh Refinement to the solid, you have to select the checkbox. You can select the type of mesh refinement from the list. By defining the FE length, mesh refinements for solids are possible (see Chapter 4.23).

If the Layered Mesh option is selected, you can directly set the number of finite element layers between two opposite surfaces. You can select Surface A from the list or use to define it graphically; the parallel Surface B is entered automatically. Afterwards, it is possible to control the number of layers in a Defined way.

Each solid has a local coordinate system. This axis system is significant for orthotropic properties, for example. Stresses and distortions are related to the local axis system as well.

RFEM displays the coordinate systems as soon as you move the pointer over a surface. You can use the shortcut menu of a solid to switch them on and off.

In the Edit Solid dialog box, you can adjust the solid coordinate system. Double-click the solid to open the dialog box. The orientation of the local axes is managed in the Axes dialog tab.

The solid's local axes x and y can be oriented to be parallel to the axes of a boundary surface, a line, a surface, or in direction of a user-defined coordinate system (see Chapter 11.3.4).