CNCCookbook: Be a Better CNC'er

Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results now.

CAM Toolpath Strategies

One of the big differentiators of the different CAM programs seems to be the flexibility and choices they give for toolpaths. There are a lot of different ways a CAM program could choose to generate a toolpath, and that choice will affect the speed and surface finish of the resulting cuts. On this page I've tried to round up as many different toolpath strategies as I could find in order to try to understand what the differences are.

It is important to note that the most sophisticated CAM programs approach the problem with the assumption that multiple specialized toolpath strategies may be used to produce the part as efficiently as possible. For example, plunge roughing may be used to rough the part, an intermediate roughing strategy such as zig-zag roughing would follow, and finally a toolpath such as two linear machining paths on crossed axes might be used to create the final finish.

An important term to understand is Tool Engagement Angle (TEA): The amount of circumference of the cutter in degrees that is engaged in cutting at any point in the toolpath. The larger the maximum TEA, the more stress is put on the cutter. Check out the Mill Surface Finish Page for more details on how cutter engagement factors in.

Toolpath Strategy Roundup

Toolpath Strategy
Pros & Cons
Between Curve Milling Generates a toolpath that will create a smoothly interpolated surface between two curves. + Convenience and ease of use.
Constant Stepover A toolpath wherein the tool follows the shape of the pocket using parallel paths that are separated by a constant stepover.

+ The simplest and most obvious toolpath strategy. This is the default approach and may not even be given a name in the CAD program.

+ Produces a very consistent and regular looking finish.

- Limited in performance due to high corner loads. The tool has to be limited on the whole path to the maximum speed that makes sense in a tight corner. See TrueMill for one method of overcoming this limitation.

Constant Scallop Height Machining See "Constant Z Machining".  
Constant "Z" Machining A strategy typically used for finishing where the toolpath tracks at a constant Z around the profile being machined. It is typically used for steep walls, with another strategy applied to other situations. Areas that are not steep are avoided by limiting the path to contact angles that range from 30 to 90 degrees.

+ Produces a pretty finish because the scallops are all the same height.

- Use is restricted to steep walls.

Helix Ramping Rather than just diving straight in this approach strategy has the tool ramp into the cut along a helical arc.  
Hole Detection A feature of the CAM program that allows it to ignore holes for most operations so that a special toolpath can be created to drill them. + Convenience and productivity
Horizontal Machining A finishing strategy that attacks all the flat areas first, and uses another more optimal strategy for the slopes.  
Linear Machining

Profiling or contouring a part using constant stepover toolpaths that are parallel in the XY plane and vary in Z as needed to follow the contours of the part. Crossed linear paths can provide a very fine surface finish to contoured parts.

Generally used for finishing passes.

Offset Area Clearing The toolpath proceeds at a constant offset around the boundaries of the part.  
Parallel Pencil Milling A variation on pencil milling (see also) where the user can specify the number and stepover of passes to be made parallel to the pencil milling pass.  
Pencil Milling

A final finishing technique primarily intended to address corners and concave areas not handled by toolpath strategies used earlier in the program. Pencil milling allows a toolpath where the cutter diameter is the same as the diameter of the feature to be milled.

Without pencil milling, or rest machining, operators used to have to manually specify the corners that needed machining. If you have powerful rest machining, pencil milling is not needed.

+ Very high surface finish.

+ Convenience and productivity

- Unnecessary complication when rest milling is available.

Plunge Roughing

A roughing technique where cutting occurs through motion only of the Z-axis, much like plunging a drill repeatedly into the workpiece. It takes advantage of the fact that most machines are far more rigid in the Z-axis and can take a much higher feed rate and/or a larger cutter when used in this way.

Plunging works best if the toolpath is orchestrated to ensure climb milliing.

+ May result in higher performance when roughing.

- Leaves behind a rough blocky surface that has to be finished out carefully.

Profile Ramping A toolpath that ramps into the cut following the profile of the part.  
Raster Finishing See "Linear Machining", it's the same thing.  
Rest Machining or Rest Roughing Rest Machining is a strategy that allows larger cutters to be used for roughing, followed by smaller cutters for finishing. It requires the CAM program to accurately keep up with what's left to be machined or "the rest of the material." + Use of larger cutters for roughing speeds cutting times.
Solid Machining Technology (SMT) SMT is a proprietary technology developed by OneCNC to smooth out toolpaths generated by that CAM program.

+ Better surface finish

+ Longer tool life

Trochoidal Machining A machining technique intended to control the TEA by moving the tool in a series of circles that step forward slowly. This causes the tool to always move along a curve of constant radius so that feed rates can be optimized for that path more easily.

+ Higher cutting speeds, longer tool life.

- Trochoidal machining is an early HSM toolpath that avoids sharp corners. The big loops can waste a lot of travel compared to newer strategies.

TrueMill, Volumill, Adaptive Clearing and other Constant Tool Engagement Angle HSM Toolpaths TrueMill is a technology that dynamically varies stepover and toolpath when cutters are near corners to limit the amount of TEA of the cutter that is engaged and thereby allow faster feeds throughout the toolpath.

+ Very high performance because the toolpath can keep the cutter working near its limits all the time. This allows shorter cutting times and longer cutter life.

+ Lower stress on cutters and the machine tool. This results in longer life and potentially greater accuracy through less flexure.

+ Less wasted travel than trochoidal paths.

- Proprietary technology is limited to SurfCAM. Take a look at Trochoidal Machining for a similar strategy.

- TrueMill paths may look odd or random, which may be undersirable from a cosmetic standpoint.

Waterline Finishing See "Constant Z Finishing"  
Zig-zag Clearing A toolpath designed to optimize the amount of straight line motion of the cutter. It is used for 3D profiling operations. In operation, the tool zig zags back and forth over the workpiece, with the z-level varying as needed.

+ Somewhat more optimal cutting speed than the more basic strategies, particularly those planar strategies that always cut in the same direction and then retract and move all the way back to start the next cut.

- Back and forth zig zags alternate climb with conventional milling. This may not give the best surface finish and will shorten tool life.



Sale Details

Featured Articles

Step-By-Step Guide to Making CNC Parts

CNC Router Cutter Types

Why Use a Single Flute Endmill?

Step and Servo Motor Sizing

The Truth About Tool Deflection

10 TIps for Router Aluminum Cutting

2 Tools for Calculating Cut Depth and Stepover

CNC Machine Hourly Rate Calculator

Special Purpose CNC Calculators

Feeds and Speeds Guide

CNC Cutter Guide

Feeds and Speeds By Material

G-Code Tutorial

  Feed Rate Calculator

Sales, and Special Deals


GCode is complicated.
G-Wizard Editor
makes it easy.

Try It!


Feeds and Speeds:
Made Easy.

Try G-Wizard



Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results now.


Start Now, It's Free!