Welcome to our 4-Part series on Hole Machining in 2 & 3 Axis CAM using MecSoft’s CAM plug-ins. The complete 4-part Guide is available to all AMS subscribers as part of your CAMJam Self-Training package. See How to Download your CAMJam Training Materials for information about CAMJam and how to reap the benefits of your AMS subscription! In part 2 of our series we explore the Hole Cutting Parameters available to each hole operation. You will learn about each hole type’s canned cycle code properties and the Cut Parameters of two 2 Axis Milling toolpath strategies that are used exclusively for cutting holes. These are 2 Axis Hole Pocketing and 2 Axis Hole Profiling. Hole Sorting Rules are also included in this section. The following 4 blog articles are included in this series:

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

 

Hole Machining Parameters

Each hole operation dialog has a Cut Parameters tab that contains all of the cycle parameters needed to define the hole. For example the Drill operation dialog includes a Drill Type selection menu that allows you to define the type of drill cycle to define. For drilling, the menu includes Standard Drill, Deep Drill, Break Chip Drill, Countersink Drill as well as four User Defined Drill Cycles. The Canned Cycle Parameters and the Hole Milling parameters are discussed in a separate section below.

Standard Drill	Deep & Peck Drill	Countersink Drill

 

Tap	Bore	Reverse Bore

The tables below list the canned cycle parameters supported by each hole type. You will notice that some parameters enable or disable other parameters. For example, in the Countersink Drill type, Countersink Diameter is enabled and Depth is disabled.

Drill Cycle Cut Parameters

Example G-Codes:

G81X1.2374Y1.2374Z-0.6443R0.25F10. G82P0X1.2374Y1.2374Z-0.1443R0.25F10. G83X1.2374Y1.2374Z-0.6443R0.25Q0.1F10. G73X1.2374Y1.2374Z-0.6443R0.25F10.Q0.1

 

Drill Cycle Cut Parameters
Parameter
	Standard G81	Deep G83	Countersink G82	Breakchip G73	User Defined
Depth			–
Add Tool Tip to Depth
Location At Top
Location At Bottom
Location Pick Top
Projects to 3D Model
Dwell Off
Dwell Time/sec
Dwell Rev/rpm
Approach Distance (R)
Countersink Diameter	–	–		–	–
Step Increment (Q)	–		–

 

Tap Cycle Cut Parameters

Example G-Codes: G84X1.2374Y1.2374Z-0.5R0.1F300. G84X1.2374Y1.2374Z-0.5R0.1Q0.1F14.667

Tap Cycle Cut Parameters
Parameter
	Standard Tap G84	Peck Tap G84	User Defined Tap
Depth
Location At Top
Location At Bottom
Location Pick Top
Projects to 3D Model
Dwell Off
Dwell Time/sec
Dwell Rev/rpm
Approach Distance (R)
Direction Right/Left
Cut Peck Depth (Q)	–		–

 

Bore Cycle Cut Parameters

Example G-Codes:

G85X1.2374Y1.2374Z-0.5R0.1F14.667 G86X0.750Y-0.750Z-0.500R0.100F14.7 G87X0.750Y0.750Z-0.500R0.100F14.7

 

Tap Cycle Cut Parameters
Parameter
	Drag Bore G85	NoDrag Bore G86	Manual Bore G87	User Defined Bore
Depth
Location At Top
Location At Bottom
Location Pick Top
Projects to 3D Model
Dwell Off
Dwell Time/sec
Dwell Rev/rpm
Approach Distance (R)
Tool Orientation	–		–

 

Reverse Bore Cycle Cut Parameters

Example G-Codes: G77X1.2374Y1.2374Z-0.5R0.1F14.667

Tap Cycle Cut Parameters
Parameter
	Reverse Bore G77	User Defined Reverse Bore
Depth
Location At Top
Location At Bottom
Location Pick Top
Projects to 3D Model
Dwell Off
Dwell Time/sec
Dwell Rev/rpm
Approach Distance (R)
Tool Orientation

 

Hole Milling Operations

For larger holes you can select from one of the 2 Axis Milling toolpath strategies that are specifically designed for cutting circular holes and pockets using mill cutting tools. These include 2 Axis Hole Pocketing, 2 Axis Hole Profiling. It should be noted here that these are not canned holes cycles. They are 2 Axis mill cutting paths that output Linear, Arc and Helix motions. Hole Pocketing combines a helical entry motion with a spiral cut motion at each cut level. Hole Profiling is a helical cut motion combined with entry and exit motion.  

Hole Milling Cut Parameters

In addition to the Location of Cut Geometry parameters, additional Cut Parameters include a global Tolerance (t), Hole Depth (H), Hole Diameter (D), Cut Direction and Helical Pitch. Hole Pocketing also includes Stepdown (Dz), Stepover (S) and the ability to add a Cleanup Pass at each cut level. Both of these operations allow you to optionally create full 360 degree helical motions and output each helix individually in the posted G-Code. The cut parameters for each operation type are listed below.  

Hole Pocketing/Profiling Cut Parameters
Parameter
	Hole Pocketing	Hole Profiling
Tolerance (t)
Location At Top
Location At Bottom
Location Pick Top
Hole Depth (H)
Depth from 3D Model
Hole Diameter (D)
Use Arc Diameter
Cut Direction
Stepdown (Dz)
Stepover (S)		–
Do Cleanup Pass		–
Helical Entry		–
Linear Entry	–
Radial Entry	–
Ramp Entry	–
Full 360 Degree Helix		–
Output each Helix Individually		–

 

Hole Sorting Rules

If you have many holes to machine in one operation, you can take advantage of the Sorting tab on each hole operation dialog. It allows you to perform a Minimum Distance Sort and Directional Sort of the holes. In Minimum Distance Sort you can specify the starting location such as Lower Left, Upper Right, etc. The program will calculate the hole machining sequence based on the distance between holes. If you have a lot of holes in a close pattern this option will keep the machining time to a minimum. If you have a lot of holes in multiple patterns you can use the Direction Sort option. This allows you to specify a Primary and Secondary Direction as well as the Traversal Pattern (i.e., Zig or ZigZag). The Sort tab is also available all Hole operation dialogs as well as many other Milling operations.

 

 

 

 

 

 

For more information:

Here is the list of articles in this series:

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control