Brick elements are four-, five-, six- or eight-node elements formulated in three-dimensional space. Brick elements are used to model and analyze objects such as wheels, flanges, and turbine blades. Brick elements have the ability to incorporate midside nodes (producing 21-node elements) and several material models.
When applying loads to a surface number of a brick part, be aware that some models may not have all the lines on the face to be loaded on the same surface number. What happens in this situation? If the model originated from a CAD solid model, all faces coincident with the surface of the CAD model receives the load regardless of the surface number of the lines. In hand-built models and on CAD parts that are altered so that the part is no longer associated with the CAD part, the surface number that is common in any three of the four lines that define a face (four-node region) or two of the three lines (three-node region) determines the surface number of that face.
These 4- to 8-node elements are formulated in 3D space, and have only three degrees-of-freedom defined per node: the X translation, the Y translation and the Z translation. Incompatible displacement modes are available only for 8-node elements. Pressure, thermal and inertial loads in three directions are the allowable element based loadings. You may also use centrifugal and nodal loads.
Figure 1: 3D Brick Element, 8-node
Figure 2: 3D Brick Element, 7-node
Figure 3: 3D Brick Element, 6-node
Figure 4: 3D Brick Element, 5-node
Figure 5: 3D Brick Element, 4-node
If you want the brick elements in this part to have the midside nodes activated, select the Included option in the Midside Nodes drop-down menu. If this option is selected, the brick elements have additional nodes defined at the midpoints of each edge. (For meshes of CAD solid models, the midside nodes follow the original curvature of the CAD surface, depending on the option selected before creating the mesh. For hand-built models and CAD model meshes that are altered, the midside node is located at the midpoint between the corner nodes.) It changes an 8-node brick element into a 20-node brick element. An element with midside nodes results in more accurately calculated gradients. This is especially useful when trying to model bending behavior with few elements across the bending plane. Elements with midside nodes increase processing time. If the mesh is sufficiently small, then midside nodes may not provide any significant increase in accuracy.
Next, select the integration order that is used for the brick elements in this part in the Integration Order drop-down menu. For rectangular shaped elements, select the 2nd Order option. For moderately distorted elements, select the 3rd Order option. For extremely distorted elements, select the 4th Order option. The computation time for element stiffness formulation increases as the third power of the integration order. Consequently, the lowest integration order which produces acceptable results should be used to reduce processing time.
When you use a Moldflow material model, use the Residual Stress (Moldflow Insight Only) drop-down to include or exclude residual stresses for your analysis. If set to Include, stresses built-up during the injection molding process are modeled. Upon ejection from the mold, the part shrinks and warps to redistribute the stresses incurred while in the mold. Your model part represents the in-mold dimensions.
If you are performing a thermal stress analysis on this part, specify the temperature at which the elements in this part experiences no thermally induced stresses in the Stress Free Reference Temperature field. Element based loads associated with constraint of thermal growth are calculated using the average of the temperatures specified on the nodal point data lines. The reference temperature is used to calculate the temperature change. Thermal loading may be used to achieve other types of member loadings. For these cases, an equivalent temperature change (dT) is used.
If this part of brick elements is using any material model except for isotropic or temperature dependent isotropic, you will need to define the orientation of material axes 1, 2 and 3 in the Orthotropic tab of the Element Definition dialog box. There are two basic methods to accomplish this.
The first method is to select one of the global axes as material axis 1. If you select the Global X-direction option in the Material axis direction specified using drop-down Menu, the orthogonal material axes follows the X, Y and Z axes:
The second method is to select the Spatial Points option in the Material axis direction specified using drop-down menu. Next you must define the coordinates for three spatial points in the Spatial point coordinates table. Next, select the appropriate index for the spatial points in the Index of spatial point 1, Index of spatial point 2 and Index of spatial point 3 drop-down menus. Material axis 1 is a vector from the spatial point in the Index of spatial point 1 drop-down menu to the spatial point in the Index of spatial point 2 drop-down menu. Material axis 2 is perpendicular to local axis 1 and travels through the spatial point in the Index of spatial point 3 drop-down menu. Material axis 3 is calculated as the cross-product of material axis 1 and material axis 2.