Manual Mesh Generation in StressCheck

To access manual mesh generation tools in StressCheck, select Class > Mesh or navigate to the Mesh tab in the Input dialog. Then, set the C/A/O/M Action to Create, the Object to the desired standard element type (Triangle, Quadrilateral, Tetrahedron, Pentahedron, or Hexahedron), and the Method to one of the below methods.

Manual (hand) meshing requires the selection of existing user-defined nodes, edges or faces. Nodes may be geometrically associative, or not, depending on the node creation method. If the nodes are geometrically associative, then the elements created from those nodes will inherit properties and assignments from the geometry, as well as be geometrically mapped. Learn more about Node Creation Methods.

Once the user has generated the sufficient node/edge/face objects, StressCheck has several methods available for manual generation of finite element meshes of the standard element types.

For an example of manually meshing a racetrack cutout, refer to StressCheck Tutorial: 3D Manual Mesh for Racetrack Cutout.

Selection Method

Elements may be created by manually selecting individual nodes. After selection of the required nodes, the element will be automatically generated.

• Triangle – select three (3) nodes in any order
• Quadrilateral – select four (4) nodes in any order
• Tetrahedron – select four (4) nodes in any order
• Pentahedron – select three (3) nodes in any order to complete the first triangle, then select three (3) nodes in any order to complete the second triangle
• Hexahedron – select eight (8) nodes in any order

The below animated example shows the manual generation of a pentahedron for Create > Pentahedron > Selection.

Individual Node Selection

If you choose the wrong node while defining an element, you may click the right mouse button to abort the generation. Alternatively, you may use the Backspace key on the keyboard, or hold Ctrl and click, to deselect the nodes you have selected by mistake. In this way you do not have to select all nodes again, only continue from where you left off.

Marquee Node Selection

It is also possible to define an element by selecting all desired nodes in one operation using what is called a marquee pick. Simply left-click and drag a box around the desired nodes. You may select nodes one at a time, two at a time, or several at a time in order to create elements. Similarly, you may cancel them in the same fashion by pressing the Ctrl key while you perform a marquee pick.

Semi-Automatic Selection in 2D

In addition to standard element creation by individual node selection, and marquee selection, StressCheck provides a facility for creating individual elements semi-automatically. If you press both the Ctrl + Shift keys as you move the cursor across the Model View, the program will automatically sense the location of the cursor, and its proximity to various nodes that have been defined in your model. StressCheck will display a candidate element connecting the nodes within the proximity of the mouse cursor that will form a valid element of the chosen type (triangle, quadrilateral). If the candidate element is the one you want, simply click the left mouse button, and the element will be created.

It is sometimes necessary to rotate or translate the model to obtain an orientation in which the candidate element can be properly identified. You may manipulate the view using the right mouse button, without leaving the element creation operation. Sometimes it is difficult to position the mouse cursor in such a way that the candidate element is the one that you are seeking. In this case, it is possible to indicate to StressCheck that you wish to identify the first edge of a 2D element, then move the cursor to complete the element. To operate in this two-step mode, simply hold the Shift key while you move the cursor over the Model View. You will see a candidate edge appear. When you see the desired edge, click the left mouse cursor. When you click the mouse, the nodes associated with the chosen edge will be highlighted. As you move the cursor, the selected edge will be preserved, and any subsequent candidate element will include this edge. When you click again, the candidate element will be created.

Sometimes even with these candidate element construction procedures, it is difficult to identify the desired element. In this case, you may wish to select some desired nodes individually, then let the automatic procedure complete the element for you. To select nodes individually, you may use either the marquee pick or individual node selection. After selecting the nodes, press the Ctrl + Shift keys and the automatic selection procedure will take over and display either the candidate edge if you have identified fewer than half the necessary nodes, or the complete candidate element if you have identified at least half of the necessary nodes. To summarize the semi-automatic element construction procedures:

• No key depressed – select individual nodes (suppress candidate element evaluation and display)
• Shift key depressed – select nodes in proximity of cursor to form first edge/face of candidate element
• Ctrl + Shift keys depressed – select nodes in proximity of cursor to produce complete candidate element.

Note: As with any multi-step construction technique, you may abort the current operation by clicking the right mouse button.

Semi-Automatic Selection in 3D

Similar to 2D, StressCheck provides a facility for constructing 3D elements semi-automatically. While creating elements with the Selection method, if you press the Ctrl + Shift keys as you move the mouse cursor across the Model View, the program will automatically sense the location of the cursor and display a candidate 3D element based on the proximity to various nodes that have been defined in your model. If the candidate element is the one you want, simply click the left mouse button, and the element will be created.

It is sometimes difficult to position the mouse cursor in such a way that the candidate element is the one that you are seeking. In this case, it is possible to indicate to StressCheck that you wish to identify the first face of a 3D element, then move the cursor to complete the element. To operate in this two-step mode, simply hold the Shift key while you move the mouse cursor over the Model View. You will see a candidate face appear. When you see the desired face, click the left mouse button. When you click the mouse, the nodes associate with the chosen face will be highlighted. As you move the cursor, the selected face will be preserved, and any subsequent candidate element will include this face. When you click again, the candidate element will be created.

As in 2D, you may select nodes individually or using the marquee pick. If you subsequently hold the Ctrl + Shift keys down, the automatic element construction will take over and display the candidate face if you have identified fewer than half the necessary nodes, or the complete candidate element if you have identified at least half of the necessary nodes. When constructing a tetrahedral or pentahedral element using the candidate face technique, the first candidate face is triangular.

When constructing a 3D element semi-automatically, the candidate element may not look valid. This is because candidate node selection is based on constructing an element with straight edges and faces. Before the candidate element is displayed however, the associativity is evaluated and the actual element using the candidate nodes is then displayed. It is not possible to actually create an invalid element, since it will first be evaluated, and then rejected if it is not valid. This technique is more efficient than evaluating the associativity for all possible candidate elements.

Note: As with any multi-step construction technique, you may abort the current operation by clicking the right mouse button.

Edge to Edge Method

If a gap between Planar elements (i.e. Triangles, Quadrilaterals) exists, then the user may select one Planar element edge, then another Planar element edge across from the selected edge, to create a new Planar element. The below animated example shows the manual generation of a quadrilateral for Create > Quadrilateral > Edge to Edge.

Face to Face Method

If a gap between 3D elements (i.e. Tetrahedra, Pentahedra, Hexahedra) exists, then the user may select an existing element face, then another element face or node across from the selected face, to create a new 3D element.

• For Create > Tetrahedron > Face to Face, select one face and then an opposing node
• For Create > Pentahedron > Face to Face, select two opposing triangular faces
• For Create > Hexahedron > Face to Face, select two opposing quadrilateral faces

The below animated example shows the manual generation of a hexahedron for Create > Hexahedron > Face to Face.

Refinement of Manual Meshes

If required, manual meshes may be refined by using h-Discretization tools. These tools are discussed in H-Discretization Overview and demonstrated in StressCheck Tutorial: Performing h-Discretization to Refine Manually Generated Meshes.

Mesh Seeding

Starting with StressCheck v12.0, manually generated nodes (and any elements meshed from these nodes) can be used to “seed” the MeshSim automesh generator. For example, nodes placed at specific intervals along a curve will be respected when the automatic meshing routine is invoked. Learn more details in MeshSim Automesh Generators.