NC-Drilling
Drill Tool Definitions
Drill tools are
defined in the same way as Milling and turning tools. NC-Tool
Lib-Define Drill Tool
Tool Section, common to all drilling tools:
Name enter a name to describe the drill. The tool table is sorted by this name so it is a good idea to keep the names consistent. The name above would be a 1/8 diameter, high-speed steel drill, with feeds and speeds set to cut aluminum.
Number the location of the tool holder within a tool holder magazine,
Correction D the offset memory location within the controller in which the radius of the cutter is stored.
Correction L The offset memory location within the controller in which the length compensation value is stored. This value is used in most multiple tool setups.
Drill Tool drills specific parameters.
Diameter Enter the actual diameter of the tool. This value is used to represent the tool size during simulation.
Length Enter the length of the flutes of the drill. This value is only used in the simulation representation.
Angle Conic Enter the included angle of the drill tip. A flat-bottomed drill is 180 degrees. Common angles are 118 degrees for drilling steel and 135 degrees for drilling softer materials such as plastics, copper, and brass. The drill tip angle is used during simulation. It may be changed within the job table if a different result is desired.
Technology
Feed normal drilling feed rate for this drill and material. Usually specified in units per time, inches per minute, inches per second, mm per minute, etc. For tapping operations, specified as units per rev, ie .05 inches per revolution for a Ό-20 thread.
Feed Retract a different feed rate to be used when withdrawing the tool under program control. This is usually specified in the same units as Feed.
Speed Spindle speed to be used with this specified tool and material. Specified as RPM.
Tapping Tool Definitions
Taps are defined in the same way as Milling and turning tools.
NC-Tool Lib-Define Drill Tool
Select
Drill Tap from the listed tool types
Tool Section, common to all drilling tools:
Name enter a name to describe the drill. The tool table is sorted by this name so it is a good idea to keep the names consistent. The name above would be a 1/8 diameter, high-speed steel drill, with feeds and speeds set to cut aluminum.
Number the location of the tool holder within a tool holder magazine,
Correction D the offset memory location within the controller in which the radius of the cutter is stored.
Correction L The offset memory location within the controller in which the length compensation value is stored. This value is used in most multiple tool setups.
Drill Tap Tool tapping specific parameters.
Diameter Enter the actual diameter of the tool. This value is used to represent the tool size during simulation. Usually the major diameter of the thread
Length Enter the length of the flutes of the tap. This value is only used in the simulation representation.
Angle Conic Enter the included angle of the tap tip. Common angles are 60 degrees for ground taps. The tap tip angle is used during simulation. It may be changed within the job table if a different result is desired.
Thread Pitch This value is the pitch of the screw thread. For a Ό-20 thread, the thread pitch is 1/20 or .050 inches.
Technology
Speed The spindle speed at which the tap will be driven. Specified in rpm.
Feed The Feed and Feed retract are automatically calculated when the Spindle speed is entered followed by a tab. This is expressed in units per minute. inches per minute, or mm per minute, etc. Changing the feeds will also change the Spindle speed.
Feed Retract a different feed rate to be used when withdrawing the tool under program control. This is usually specified in the same units as Feed.
Drilling
Vector supports a selection of fairly standard canned Drill cycles. These can be posted to iso g-code or Heidenhein formats. The tools used for canned cycles, whether drills, or boring bars are defined as a drill tool for purposes of Drill Cycle usage. Taps are defined separately as shown earlier in this section.
To create toolpaths for drilling, the geometry construction is normally one or more point entities (Draw-Point). Arcs can also be used for drilling.
Points drawn in an arc using Draw-Arc-Circular Hole Pattern, with Radius=0.
If all the positions are to be drilled to the same depth, the points may be drawn with Z=0 and the depth can be specified within the drill dialog. If the holes are to be processed to different depths, draw ALL points at the desired Z depth. In this case the first hole can be drawn at z=0 or at the desired depth, but its depth must be specified on the NC-Drilling dialog. The post processor can be modified to always use different drill depths, but the default posts will have the first point specified by the NC-Drill depth and the remaining points will be specified by a modal Z value, unless they are different from the first hole depth. If the target machine controller does not support multiple depths within the same Drilling cycle callout, separate canned cycles can be used for each hole, or a Connect at Z can be used to create a milling tool path that will use G01 and G00 moves to drill any number of holes at different depths. In order to use connect at Z method, the points must be placed at the desired depth in Z, prior to using connect at Z. This toolpath can be simulated if it is turned into a milling job using NC-Jobs-Define Job Mill
The Drill cycles are: NC-Drilling-Drill Which generates a G81 cycle in ISO G-code
Job Enter a Name for this process step that describes the operation, such as
Drill 1/8
.25 deep
Tool Select a tool from the Drill tool library. If no tools or the wrong ones are listed, click ADD and create any needed tools, (or using NC-Tool Lib-Define Drill tool to add a new tool), or NC-Tool lib-Import Tool Table to load a predefined tool table.
Technology These values are defined when the tool is defined and are filled in when the tool is selected from the tool table. Entering new values for Feed, Feed Retract, and Spindle speed may change the technology settings, or they may be modified directly within the Job list.
Drill Operation
Depth is the total depth to drill the hole, including the conical tip of the tool. Will be used for all holes selected, unless they have been drawn with differing Z depths. Rule of thumb: To drill to full diameter depth, add about 1/3 the diameter for a 118 degree.
Z-Rapid height in Z for the first motion
Z-Retract Z retract height above the workpiece
Z-Safe Safe Z height between Drill points
These values are all available for output to the post processor, but may not be required for all machine controller canned drilling cycles.
After the parameters are all entered, Click OK.
The Drilling toolpath object is created and the job step is added to the Job list. The operation may be edited and deleted if needed from the NC-Jobs-Job Table
The drill will be shown if the job table is simulated and if the NC button is clicked, the Drilling cycle will be generated into the NC editor. Drilling depth as well as any of the other drill cycle parameters can be modified directly from the job table. The Vector drawing of the drilling toolpath is updated when the drill depth is changed in the job table.
With the variations noted below, all the Drilling cycles, including tapping and boring are processed in the same manner.
NC-Drilling-Drill Dwell, which generates a G82, canned cycle in ISO G-code
The Dwell time is added to the available parameters, enter the time for the tool to dwell at the bottom of the hole for chip breaking.
NC-Drilling-Drill Peck, which generates a G73 for complex pecking or a G83 for simple pecking. The code may be configured in the post processor, depending on the requirements of the machine controller.
Both dwell and peck parameters are available for entry with this canned cycle. The Step DZ is the first peck depth, Reduce DZ is the amount by which the second and each subsequent pecks are reduced, and Minimal DZ is the amount of all pecks after the reduced DZ has all been utilized. In the G83 usually only the Step DZ is implemented. However, this varies greatly by controller and can be easily customized within the Vector NC configuration of the post processor.
Peck drilling motion is not currently implemented in the simulator, but the tool and the total material removal, including the conical tip and any gouging are shown.
Tapping
NC-Drilling-Tap Left or NC-Drilling-Tap Right
All Drill Operation values are the same as for drilling cycles. Left and right hand tapping are differentiated when the g-code is generated. The thread pitch and feeds are selected from the Tap tool parameters.
Boring
Options for boring are:
NC-Drilling-Boring
NC-Drilling-Boring Dwell
NC-Drilling-Boring Stop Manual Retract
NC-Drilling-Boring
Dwell Manual Retract
These are all standard Fanuc canned cycles and use the same parameters described for Drilling and tapping cycles.
Fine Boring
Fine Boring uses the same parameters as Boring, with the addition of a spindle stop, and offset. This permits withdrawal of the boring tool from the hole without leaving a witness mark from the tool tip.
Available cycles are:
NC-Drilling-Fine Boring
NC-Drilling-Fine Boring Back
Use Shift DX or Shift DY to offset the tool from the hole center coordinates after the spindle stops.
Dwell time can be used to permit the spindle to come to a full stop, prior to tool retraction.