Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

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 this fourth and final installment of our series we explore posting your Hole Machining operations to G-Code. This includes posting Hole Operations to canned cycles and how to optimize the cycle output to reduce files sizes by up to 75%. If your controller does not support canned cycles, we also cover user-defined hole cycles and the ability to post your hole operations as linear motions. 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 3: Output Control

Hole Machining Output Control

By default, hole machining operations including Drill, Tap, Bore & Reverse Bore are posted out as canned cycles. See Hole Machining Parameters above for more information on which canned cycles are used. If your controller cannot handle canned cycles you can output these hole operations as linear motions. There are also options within each post definition file for controlling how your posted G-Code is formatted for hole operations.

Posting Canned Hole Cycles

By default your hole operations (Drill, Tap,Bore and Reverse Bore) are posted out as canned cycles. See Hole Machining Parameters above for more information on which canned cycles are used. If you are not seeing canned cycle codes in your posted file, go to the CAM Preferences dialog. Select Machining from the left side of the dialog and look for the Drill Cycle Output section. Make sure the box for Always output as linear motions is unchecked. For more information about posting canned cycles we have a guide called Post-Processor Generator (PPG) Decoded. You can download this guide from our 2019 Printed Media Guide.

Optimizing Hole Cycles Output

If your part has many holes that are being output as canned cycles there is an option to Optimize your Cycle Output. This option is located in your post-processor definition file. It will reduce the amount of code in your G-Code file for canned cycles. For more information about this option you can refer to the Post-Processor Generator (PPG) Decoded guide. You can download this guide from our 2019 Printed Media Guide.
Fixture Plate requires over 85 pre-drilled holes
Drill Cycle Output
Optimized Drill Cycle Output Reduces posted code by 75%

User Defined Hole Cycles

If you need to post a specific line or lines of G-Code for a hole cycle you can use one of the User Defined Cycles. Each hole operation type (Drill, Tap, Bore and Reverse Bore) has several user defined cycles that can be utilized. Here is the basic procedure for a user defined Drill cycle. The procedure is similar for Tap, Bore and Reverse Bore cycles: 1. Create the toolpath operation for the Drill cycle. 2. From the Drill Type selection menu on the Cut Parameters tab, select User Defined Drill1. There are four to choose from. 3. Complete the remainder of the Drill operation dialog and Generate the toolpath. 4. Edit your post definition by going to the Program tab and select Post. 5. From the Set Post-Processor Options dialog, make sure your desired post is selected and then pick the Edit button (to the right of your post selection) to display the Post-Processor Generator. 6. From the left side, expand the Cycles selection and pick the corresponding User Defined Cycle. In this example we used User Defined Drill1 so select User Defined Drill Cycle 1 from the list of Cycles. 7. Use the dialog to enter information about your cycle including the Cycle G-Code, Cycle Code and other options specific to the cycle type. 8. To add the User Defined Cycle to your existing post definition pick Save. Optionally you can pick Save As and save the post definition file to a different file name. 9. Post your hole operation and review your G-Code, adjust as needed.

Post Hole Operations as Linear Motions

If your CNC controller does not support canned cycles you can post your hole operations as linear motions. Go to the CAM Preferences dialog. Select Machining from the left side of the dialog and look for the Drill Cycle Output section. Check the box to Always output as linear motions.
CAM Preferences > Drill Cycle Output (as Linear Motions)

For more information:

Don LaCourse

Don LaCourse

Don LaCourse is an Application Engineer with MecSoft Corporation. Don brings over 20 years of experience in CAD/CAM operations in both automotive and mold design applications. Don also has extensive experience in documenting CAD/CAM products and is actively involved with writing the on-line help as well as creating training tutorials for MecSoft's products.
Shopping Cart