1. CAM与自动编程
封志明

2. --Chapter IX-- IX、 Drilling Drilling Operations Overview
Drilling Geometry
Drilling Cycles
Cycle Parameters
Cycle Operation Example
Mechanical University

3. To be able to Create a Drilling Operation.
Chapter IX
To understand the Drilling Operation.
To understand the Drilling cycles and cycle parameters.
Objectives
To be able to Create a Drilling Operation.

4. 9.1 Drilling Operations Overview
9.1.1 Drilling Operations Introduction
Drilling
Use Drilling operations to machine simple holes. For more complex holes such as counterbore holes or undercut holes, consider using milling operations.
Drilling Operation

5. 9.1 Drilling Operations Overview
Parameters
Geometry
Depth
Minimum Clearance Distance
Dwell
Break Chip
use a point to point processor to generate tool paths
drill geometry parent groups

6. 9.1 Drilling Operations Overview
9.1.2 Drilling Operations Subtypes
Tab9-1. Drilling Subtype
Subtype
SPOT_FACING
SPOT_DRILLING
DRILLING
PECK_DRILLING
BREAKCHIP_DRILLING
BORING
REAMING
COUNTERBORING
COUNTERSINKING
TAPPING
THREAD_MILLING
MILL_CONTROL

7. 9.1 Drilling Operations Overview
9.1.3 Drilling Tool

8. 9.1 Drilling Operations Overview
9.1.3 Drilling Tool

9. 9.2 Drilling Geometry 9.2.1 Drill Geometry parent groups
Use Drill Geometry parent groups to manage the drill geometry. If drilling operations are associated to Drill Geometry parent groups, that same geometry rather than a new one can be used for each operation.

10. 9.2 Drilling Geometry 9.2.2 Drill Geometry subtypes Subtype
① Specify Holes
② Specify Top Surface
③ Specify Bottom Surface
To select the hole geometry and specify parameters.
To define a face or plane to which all points are projected.
To define the hole depth in the model. You must select a face/plane, /arc to specify the bottom surface.

11. 9.2 Drilling Geometry 9.2.3 Create Drill Geometry Parent Group Steps
① On the Insert toolbar, click Create geometry   , or choose Insert→Geometry.
② In the Create geometry dialog, in the type group, select drill from the list.
③ In the geometry subtype group, click DRILL_GEOM
④ In the Location group, from the Geometry list, select a geometry parent group.
⑤ Click OK.
⑥ In the Geometry group, click Specify Holes  .
The Point dialog box appears.
⑦ Click Select. Select the edge of the holes.
⑧ Click OK until you close all the dialog boxes.

12. 9.2 Drilling Geometry 9.2.4 Specify Holes Specify Holes
Specify Holes is applied to select the hole geometry and specify parameters.

13. 9.2 Drilling Geometry
9.2.4 Specify Holes 
Specify Holes

14. 9.2 Drilling Geometry 9.2.4 Specify Holes Select
Opens a selection dialog box to let you select geometry that represents the top of the hole. When that dialog box is open, you can select the geometry in the graphics window, by name, or using any of the available options.

15. 9.2 Drilling Geometry 9.2.4 Specify Holes Append Optimize
Adds points that you select to previously selected drill geometry.
Opens a dialog box where you can set options to optimize tool travel to reduce the length of the tool path.
Omit
Ignores points that you select on previously defined drill geometry.

16. 9.2 Drilling Geometry 9.2.4 Specify Holes Avoid
Lets you specify Tool Clearance over fixtures or obstacles within the part. You must define a Start Point, End Point and Avoid Distance. Distance represents the distance between the part surface and the tool tip.
Reverse
Reverses the order of previously selected GoTo points. You can use this option to perform back-to-back operations.

17. 9.2 Drilling Geometry 9.2.4 Specify Holes
Arc Axis Control
Display apply to display the tool axis orientation of arcs and holes by Single or All.
Reverse reverses the tool axis orientation for selected arcs and holes.
The Arc Axis Control is used to reverses the tool axis orientation for selected arcs and holes in sheet bodies.

18. 9.2 Drilling Geometry 9.2.4 Specify Holes Rapto Offset
Opens a dialog box where you can specify a RAPTO value to each selected point, arc, or hole. The Rapto Offset is the location where the feed rate changes from Rapid feed rate to a Cut feed rate.
The RAPTO value can be positive or negative.

19. 9.2 Drilling Geometry 9.2.5 Specify Top surface
Top Surface is used to define a face or plane to which all points are projected. It can be an existing face of the part, or an ordinary plane. If Top Surface is not specified, the NX defaults to the location of selected point. Your drilling feed rate starts at the minimum clearance.

20. 9.2 Drilling Geometry 9.2.6 Specify Bottom surface
Bottom Surface is used to define the hole depth in the model. You must select a face, a plane, or an arc to specify the bottom surface to drill.

21. 9.3 Drilling Cycles
Drilling Cycle
A drilling cycle describes the machine tool movements necessary to perform point-to-point machining functions, such as drilling, tapping, or boring.

22. 9.3 Drilling Cycles Characteristics of cycle types
No Cycle, Peck Drill, and Break Chip do not output CYCLE/ commands in the tool path; the motion is simulated with GOTO points.
Standard Cycle options output a CYCLE/ command at each of the specified CL (Cutter Location) points.
Standard Drill, Standard Drill Csink, Standard Drill Deep and Standard Drill Break Chip output canned cycles and are the equivalent of No Cycle, Peck Drill and Break Chip which output simulated motion.

23. 3. Drilling Cycle 9.3 Drilling Cycles
No Cycle
Cancels any active cycle. If no cycle is active, when you generate a tool path, the tool motions are generated in the following sequence:
The tool moves to the first operational clearance point at the Engage Feed Rate.
The tool moves along the tool axis at the Cut Feed Rate to a point that allows the tool shoulder to go beyond a selected Bottom Surface.
The tool is retracted to the operational clearance point at the Retract Feed Rate.
The tool moves at the Rapid Feed Rate to each subsequent operational clearance point. If a Bottom Surface is not selected, the tool feeds to each subsequent operational clearance point at the Cut Feed Rate.

24. 9.3 Drilling Cycles Peck Drill
Generates a simulated peck drilling cycle at each selected CL-point. A peck drilling cycle consists of a series of drilling motions into and out of a hole at progressive intermediate increments. The software uses GOTO/ command statements to describe and generate the required tool motions in the following order:
The tool moves at the Cycle Feed Rate to the first intermediate increment.
The tool moves from the hole to the operational clearance point at the Retract Feed Rate.
The tool moves at the Engage Feed Rate to a clearance point above the previous depth.
The tool moves at the Cycle Feed Rate to the next intermediate depth which you set using the Increment option. The increment can be None, Constant, or Variable.

25. 9.3 Drilling Cycles Break Drill
Generates a simulated Break Chip drilling cycle at each selected CL-point. The Break Chip drilling cycle is identical to a Peck Drilling cycle with the following exception: after each drilling increment, instead of generating a full retract motion out of the hole and a return motion back to a Distance above the previous depth, the software generates a Retract motion to a point that is the Distance above the current depth.
The tool moves along the tool axis at the Cycle Feed Rate to the first intermediate increment.
The tool moves back from the current position at the Retract Feed Rate to a clearance point above the current depth, defined by the Distance prompt. (see the caution below.)
The tool moves at the Cycle Feed Rate to the next intermediate depth.
The tool positions itself to subsequent operational clearance points at the Rapid Feed Rate.

26. 9.3 Drilling Cycles Minimum Clearance
The Minimum Clearance distance determines how the tool is positioned before entering the material.
If a Clearance Plane is not specified, the tool positions to the next hole at the rapid feed rate directly to the specified Minimum Clearance distance above the part surface.
If a Clearance Plane is specified, the tool moves at the rapid feed rate from the Clearance Plane to the specified Minimum Clearance.

27. 9.4 Cycles Parameters
Cycle parameters define exact tool motions and conditions such as feed rates, dwell times, and cutting increments. The dialog varies slightly as the different Cycle Type.
If you want to vary any of the cycle parameter values, a Cycle Parameter Set for each hole or group of holes can be created. You can have up to five parameter sets per cycle.

28. 5. Cycle Depth 9.4 Cycles Parameters
Opening the Cycle Depth dialog box where you can specify the depth of cut using one several options. This value represents the total depth of a hole from the part surface to the tool tip.

29. 5. Cycle Depth 9.4 Cycles Parameters

30. 9.4 Cycles Parameters Cycle parameters define Feed Rate
Specify the transit speed of tool while cutting. The current Feed Rate Units and Value are displayed.
Dwell
set the tool delay at depth of cut by number of seconds or revolutions.
Option
Turns on or off machining characteristics that are unique to a particular machine
CAM
Specifies a preset CAM stop position for tool depth for machine tools with no programmable Z-axis.

31. 9.4 Cycles Parameters Cycle parameters define Csink Diameter
Set the diameter of a countersink hole.
Entrance Diameter
Specify the outside diameter of an existing hole which is to be enlarged by a countersink operation.
Increment
Specify the dimensional value of one of a series of regular consecutive cuts to progressive depths used in Peck and Break Chip drilling operations.
Rtrcto
Specify a retract distance. The distance is measured along the Tool Axis, from the Part Surface to a point to which the tool retracts after feeding to depth.

32. 9.3 Cycles Parameters Cycle parameters define Step Values
Specify the dimensional value of one of a series of regular consecutive cuts to progressive depths used in Standard Drill, Deep and Standard Drill, Breakchip cycles.

33. 9.5 Drilling Operation Example
Drilling Part Model
Create Drilling Operation
Drilling Operation Path

34. THANKS
封志明/机械工程学院
2019年4月6日