About Expert Machinist
A typical Expert Machinist process may contain the following basic steps:
1. Set up the NC Model. Bring in the reference model and create stock.
2. Set up the database. It may contain such items as machine tools, cutting tools, fixture configurations, or machining templates. This step is optional. If you do not want to set up all your database first, you can go directly into the machining process and later define any of the items above when you actually need them.
3. Define an operation. An operation setup may contain the following elements:
◦ Operation name
◦ Machine tool
◦ Program Zero (coordinate system for CL output)
◦ Stock material specification
◦ Fixture setup
◦ FROM and HOME points
◦ Names used in Cutter Location (CL) data output and PPRINT
◦ Operation comments
You have to define a machine tool and a Program Zero coordinate system before you can start creating machining features. Other setup elements are optional.
4. Define the machining features for the specified operation. Machining features establish what material needs to be removed from the stock to achieve the reference model geometry. Each closed volume of material to be removed comprises a separate machining feature.
Define the machining features in the order you want them machined (one exception: create an Entry Hole feature after you have created the closed feature for which you need it). As you define machining features, the system allocates the appropriate material to be removed, and calculates the subsequent feature geometry based on existing machining features.
5. Create tool paths for each machining feature. Once the features are defined, you can machine them, that is, create the appropriate tool paths, at any time and in any order. You can also machine the features by applying predefined machining templates. These templates represent certain frequently used machining strategies; each strategy contains a complete set of the machining options and values that you would normally define when machining a feature.
6. After you have defined all the machining features and created the appropriate tool paths, output the complete operation to a CL file and postprocess it, or output the tool path data directly in the MCD format.
Modal Settings
Most of the machining setup elements are modal: that is, all subsequent machining features will use this setting until you explicitly change it. Among those are:
• Operation setup (including the machine tool and Program Zero coordinate system)
• Tool (provided the tool type is compatible with the machining feature type)
• Program Zero coordinate system within the machining feature (for the first machining feature, the Program Zero coordinate system specified at the time of setting up the operation will be implicitly used, unless you explicitly specify another one)