SolidCAM V10 NC software works within the SolidWorks CAD program.
Together, they make a handy associative design and NC package. SolidWorks lets users design parts, import geometry, and manage data, while SolidCAM provides an easy-touse, modestly priced, NC program that packs a broad range of competitive machining functions. Although it's general-purpose CAM software, it supports all aspects of making holes, two to five-axis and high-speed milling, five-axis positioning, tombstone machining, basic turning, and wire-EDM.
A few advanced features include trochoidal milling, plunge roughing, collision calculations that include the holder, 3 + 2 machining, rest-material machining, and the automatic setting of coordinate systems. That's a lot. So this initial review focuses on the basic machining functions.
For starters, all machining operations are defined, calculated, and verified without leaving the CAD environment. And 2D and 3D geometries for machining are associated to their CAD model. So when geometry defining a machining operation changes, the NC program updates machining operations for the new geometry.
The software is said to be process oriented and knowledge based. This means users create process templates and reuse them for similar tasks. Machining templates, for example, deal with operations such as threading, face and rest milling, and floor and wall machining.
When designers change CAD models, notifications appear in V10. When changes are subtle, the model-compare function pinpoints differences in before and after models. PDM records who made changes, when, and why.
CAD models can be imported from a wide range of formats through SolidWorks, which makes the geometry immediately accessible in V10. Such access includes feature trees, dimension tolerances, GD&Ts, surface finish symbols, sketch entities, notes, and other items related to product definition.
V10 supports part and assembly environments, as does SolidWorks. In assembly mode, jigs and fixtures appear along with parts to be machined. And several parts can be machined at the same time.
Launching V10 leaves CAM Manager and CAM functions at screen left. For each operation, reference is made to machining strategy, tool, and geometry. As an option, the tool sequence that machines a part can be listed in the tree and can stay on screen at all times. The NC software lets users change the order in which tools are employed by manually dragging and dropping entries in the tree. Clicking on an operation brings up dialogue boxes for selecting a machining strategy or entering machining parameters.
V10's tool library contains cutting tools, holders, and tool assemblies. The software accepts customer-specific cutting data to calculate recommended speeds, feeds, and cut depths. Tools can be loaded from the library or defined interactively.
The NC software also determines coordinate systems for parts and generates optional home positions. Users select the most appropriate one.
The NC's 2.5-axis milling supports drilling, profiling, and pocketing. It has canned drill cycles. Machining is done on tessellated solids or surface models, a common technique for minimizing gouges. Stock models for machining can be defined using any 2D contour or 3D model. The stock model can also come from a target model.
V10 selects machining strategies for volume milling and roughing. It generates in-process models to track excess or uncut material. Users typically rough level by level and then apply either a zigzag or one-way-only cutting pattern for finishing. The software recognizes flat areas, so they can be finished to their final depth while material is left on other areas.
Tools enter outside openings on models to avoid plunges. However, users are always in control. Roughing and reroughing material left behind can be done in one command.
Rest machining, a roughing operation, cuts only material that could not be reached by a previous tool. In 2D operations, the amount and location of remaining material is computed on original stock, final part model, toolpaths generated, and cutting tools that have been employed. After each successive machining step, the rest material is updated. Rest-material functions are available for 2.5D, 3D and 3 + 2 multisided machining, and to some extent when five-axis machining.
V10 supports plunge roughing, which can be appropriate for roughing large parts of soft materials. The software can rough by column or in steps. Trochoidal cutting, a relatively new and advanced machining strategy, is used with other strategies when roughing deep material. It uses a circular cutting motion partly in and partly out of the material.
A cutting tool can enter material on either a linear or helical path. The software is smart enough to alter the helical-path diameter to dodge obstacles. When necessary, V10 straightens the helix to a linear entry path to avoid an obstacle. The software needs only one model to machine different sides of a part. Some NC program needs separate models for each side.
Knowledge-based machining has a big role in V10. Standard machining processes can be defined and reused. Rules can be added as they arise. For instance, a rule could determine a spot drill depending on hole size or material. This automates programming, saves time, and adds consistency. Standard templates come with the software and users can make more. Templates can be set for almost any operation including thread milling, corner finishing, rest milling, and pocketing with a drill entry. Processes include parametric definitions, such as downsteps, stepovers, and surface offsets. Pocketing in prismatic parts, a common operation, takes only one button. V10 analyzes the model and recognizes pockets and profiles using constant-Z machining. For instance, cutting might be done level by level when thin walls are present. The software uses circular, contour, zigzag, or one-direction cuts. V10 supports pocketing in any order, an unlimited number of islands, island cleanup options, high-speed pocketing, contoured-wall pocketing, and open or closed pockets.
When machining a mold with holes, such as those for ejector pins, SolidCAM can turn off hole features or cover holes with a surface. This machines the surface but without the holes. And because drill cycles are sorted by levels, all operations needed to create threaded holes can use the same subroutine.
New users will find it useful to see machining strategies and operations listed in a dialogue box. SolidCAM includes graphics within the help function, but they are not available as part of the strategy or parameter dialogue boxes.
SolidCAM shines in tombstone machining. Parts can be placed anywhere on the tombstone which is just a big foursided part holder that looks like a tombstone and the software finds a home position. The function can machine multiple copies of the same part on a single face of the tombstone, or run through several machining operations for another part on another face. The software can mill in 2D and 3D on the same or multiple parts.
The software has few drawbacks. For instance, it doesn't run stand-alone nor does it have an API for customization. The software does not yet support four-axis lathes, subspindles in mill-turn functions, or parameter-associated graphics in dialogue boxes. And when the software is computing, other functions are inoperative.
Third-party partners to the NC include MachineWorks for machining simulation and toolpath verification, and Module-Works for five-axis machining. Product support comes from resellers and the SolidCAM Web site. A demo version of Solid-CAM let users see toolpaths and dialogue boxes but does not generate G-code.
SolidCAM comes from SolidCAM Ltd., Israel (Solidcam.com).
Mr. Christman is an NC software reviewer and consultant with Cimdata Inc., Ann Arbor, Mich. (cimdata.com).