Contouring Cycle & Cutter Compensation

When machining 2D profiles, nowadays almost every machine control provides the functionality of automatic cutter compensation (G41 - comp left/ G42 - comp right / G40 - cancel comp, or equivalents). This is a function that lets the control calculate the offset toolpath based on the profile that is specified in the NC code. The offset amount (tool radius) is normally specified somewhere in the controls memory (compensation of offset register), often together with other tool related data. The big advantage of this approach is that changes to the offset value are done directly on the machine without editing the NC code. This is very practical when making adjustments to compensate tool wear, handling machining tolerances, or switching to a tool with different diameter. On the other side there are some important restrictions. For example the machined profile may not contain linear or arc entities that are smaller than the defined tool radius. Unfortunately this is not always possible. Just imagine importing CAD data, where nobody knows what kind of entities the profiles include. There it would be very time consuming to check every profile element. Therefore EZCAM provides three different ways to machine a profile using the contouring cycle.

 

  1. Tool Radius Offset computed by the Software

The EZCAM system computes the offset toolpath when posting the NC code without any cutter compensation commands (G41/G42/G40). This is often used for multi-pass roughing, simple contouring without close tolerances, or basically when there is no need for adjustments on the control during machining. The Offset Direction setting specifies the direction that the tool will be offset while the Cutter Comp is always Off. For multi-pass contouring use Total Stock and Cut-Step with an optional Stock Allowance on the profile to be removed with a subsequent work step. In addition all combinations of Lead and Ramp moves can be applied without restrictions.

 

 

Click here for graphic Example

= Path Curve

= Verified Toolpath / Posted NC-Code

= Optional Stock Allowance

 

 

  1. Combination of Software Offset & Cutter Compensation

The EZCAM system computes the offset toolpath together with posting cutter compensation commands (G41/G42/G40 or equivalents) when creating the NC code. This is often used in cases where difficult profiles with undercut areas are machined in single passes. Although the tool radius itself is already offset by the software, it is still possible to apply small offset adjustments directly on the control. The Offset Direction and Cutter Comp settings are both set to the direction that the tool will be offset. The offset value (tool radius) is derived from the Diameter setting while the controls offset register number is sometimes connected to the tool number or the Comp # setting (depending on control type). Toolpath verification and display is same as previous paragraph #1 (see graphic example above).    

 

Rules to follow when using Software Offset & NC Control Cutter Compensation:

  1. Cutter Compensation on Machine

The EZCAM system does not compute any offset toolpath, but posts the exact coordinates of the machined profile together with corresponding cutter compensation commands (G41/G42/G40 or equivalents). This is often used for single-pass contouring when machining profiles with close tolerances. The offset amount (tool radius + tolerance shift) is specified in the controls memory (compensation of offset register) allowing computation of the offset toolpath. The offset register number is sometimes connected to the tool number or the Comp # setting (depending on control type). Cutter Comp setting defines offset direction while the Offset Direction is always Off. Use of Stock Allowance is optional.

 

Click here for graphic Example

= Path Curve

= Posted NC-Code

= EZCAM verified Toolpath / NC-Control generated Offset Toolpath

= Optional Stock Allowance

 

 

 

Rules to follow when using NC Control Cutter Compensation:

Important

Please read the rules listed above carefully. It may also be a good idea to consult the particular controls programming manual for additional information (expl: special approach/retract patterns, etc) on how to use cutter compensation.