Supersurf:
Introduction
Supersurf allows you to create and mesh three-dimensional surfaces. With Supersurf, you are able to model relatively complex surfaces using Non-Uniform Rational Basis Splines (NURBS). Supersurf compliments Superdraw II in providing a complete basis for subsequent decoding. Many of the menus are the same as in Superdraw II, and several of the surface construction methods are similar to the mesh construction methods available in Superdraw II. Most options related to surfaces are located in the Construct menu and most modification options are located on the Modify menu.
Supersurf supports the powerful and general NURB surface representation which can exactly represent quadric surfaces including cylinders and generalized surfaces of revolution. NURB surfaces are supported in the IGES format and are becoming the standard surface representation for many CAD/CAM systems.
NURB surfaces can be imported from IGES Mesh or constructed from lines, arcs and splines. The lines, arcs and splines can be created and modified from within Supersurf or Superdraw. Surfaces are modified by changing the construction curves and re-creating the surface.
A 'Quick msh" option can be used to create a finite element mesh from a model constructed of surface patches. You can specify a default mesh density for unassigned edges and then add mesh edge specifiers to the edges of surfaces. This defines the FEA mesh density for a Superdraw II line representation of the mesh. By transferring to the meshed model in Superdraw II, you can add forces and boundary conditions to complete the FEA model. One of the main advantages of using Surfaces is that the model can easily be re meshed with a higher density by simply changing the default mesh density and mesh edge specifiers. For proper intersecting, surfaces which share a common edge must also share the same edge end points along that edge.
The "Display" option of the Construct menu allows you to control the density of the tessellation lines. Tessellation lines are the lines used to represent the surface as a mesh. They break the surface into rectangular or triangular patches. The endpoints of the patches occur on the surface and the straight lines approximate the curved shape of the surface. This menu also lets you hide all lines, arcs, circles and splines so that only the surfaces are visible.
Since two-dimensional views of three-dimensional objects can be confusing, options which create shaded views and cut-views have been included in the "Construct:Display' menu. This option allows you to view only that the part of surfaces that fall above the cutting plane, within a fixed size band just below the cutting plane or below the cutting plane.
2. Construction and Modification
Supersurf provides several methods to create NURB surfaces. Regardless of the method of construction, all surfaces are stored internally as NURB surfaces. Some of these methods, like 2-obj, Patch and 3-Patch are similar to the Superdraw II mesh construction methods; however, they create slightly different surfaces. For example, the Superdraw II "2 object" mesh command creates ruled surfaces by linearly connecting points an equal fractional distance along each object. The Supersurf "2-obj/t" command creates a ruled surface by linearly connecting points that correspond to the same parameter in the NURB representation of the curves.
The construction methods generally far into two categories: interpolating methods and sweeping methods. The 2-obj/t, Patch/t, 3-patch/t and Multi- methods are used to interpolate between curves to form surfaces. The Tabulated, Sweep, Revolve and Helical methods arc designed to sweep a generator curve along a specific path. Only for the tabulated surface is the generator curve rigidly translated in the direction specified by the path curve without being rotated in space. The other sweep methods try to reorient the generator curve so that the relationship between the generator curve and path curve tangent remain the same.
2.1 Construction Curves
For all construction methods, you arc prompted to select the curves that are used to define the surface. These curves can be lines, arcs, open splines or edges of existing surfaces. Using the edge of an existing surface can be very convenient when creating multiple swept surfaces that arc connected together.
Closed splines and circles should be converted into open curves before being converted into surfaces. To convert a closed curve to an open curve, you can add a construction line across the curve and then use the "Modify:lntcrscct" command to intersect the curve based on the construction line. Using this method, you have full control over the surface connection between the curves (at least at the intersection points). After creating the surface, you can use the "Modify:Delete" command to remove the construction line used for the intersection operation.
When using closed curves in parallel planes, one construction line can often be used for all the curves. Use the 'Intersect:All' flag so that all curves intersected by that line can be divided in one step. Remember that the intersect command is based on the current view, so you will want the view plane parallel with the planes of the curves to be intersected.
COMBSST: combining a brick model with a beam or plate model.
COMBSST is an Algor utility which helps users combine two decoded models into one model. The following paragraphs describe in detail how to avoid pitfalls when trying to combine elements using COMBSST.
Type 2 beam elements have stiffnesses defined for all six degrees of freedom at each node (unless end releases are used to remove some stiffnesses). Type 5 brick elements have only translational degrees of freedom with stiffness. Since brick elements rotate by translation, all rotational degrees of freedom are fixed.
If a single beam (beam1) is grafted onto a brick root model (brick1), matching at one node only using the command "COMBSST:brbe:brick1:beam1," the shared node has brick fixity by default in the brbe model of ( 0 0 0 1 1 1 ) which globally fixes the beam for all rotations at that node. No moment loading from the beam will be transmitted into the brick. A beam with a pure moment loading on the free end would show stress at both ends and displacements at the free end and the brick would show neither stress nor displacement - it never sees the load at all (see Model A above).
If the same two models are combined so that the beam fixity ( 0 0 0 0 0 0 ) dominates at the shared node by using the command "COMBSST:bebr:beam1:brick1," then the beam has a pin joint where it touches the brick and is completely free to rotate. During analysis, the Static Stress Analysis Processor (SSAP0) quits with the message "model not tied down enough" and prints the equation number of the troublesome node.
Solving the Problem
The proper rule of thumb is closer to "beams first" when combining this model. Normally, the element types having the most degrees of freedom per node should predominate when using COMBSST. However, in the beam/brick example depicted above, the beam model has to contact the brick model at at least three nodes not lying in a straight line to couple all rotations between the two models.
One way to do this is to put a two-toed foot of beams on the beam model where each of the two toes goes to separate brick nodes, so that any moments in the beam are transmitted as couples to the contacted brick nodes. It is likely to have extra unrealistic stiffness where both beams and bricks overlap as though the material there was double strength and double density. While this effect can be kept to a tolerable level by care in modeling, it is probably not wise to place such element type transitions in critical stress areas of a model.
Some Tips to Consider When Using COMBSST
