CAM Features: Toolpaths for CNC, Rest Machining, and More
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.
Choosing the right toolpath is one way to improve the efficiency of the program. Once you exhaust the possibilities of toolpaths and options on your CAM software, the next level of optimization is to tackle the hand optimizing the g-code.
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 High Speed Machining page for more details on how cutter engagement factors in.
CAM Features & Toolpath Strategies
CAM & Toolpath Feature
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
|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
+ May result in higher performance when roughing.
– Leaves behind a rough blocky surface that has to be finished
|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
|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
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
3d toolpaths are more specialized. We have a great article with full details on 3d CAM Toolpaths.