QCAD.org Forum

Is there a way to generate a tool path cutting in both directions? Example, if I cut .5 inches off from 0,0 to 5,0 at .1 per pass, it generates a path that only cuts in one direction. Examples shown

G0 G90 X0.0 Y0.0
Z0.0
G1 F0.005 Z-0.1
X5.0 Y0.0
Z0.25
X0.0 Y0.0
Z-0.2
X5.0 Y0.0
Z0.25
AND SO ON
VS

G0 G90 X0.0 Y0.0
Z0.0
G1 F0.005 Z-0.1
X5.0 Y0.0
Z-0.2
X0.0 Y0.0
Z-0.3
X5.0 Y0.0

Milling a piece is done or in conventional mode or in climb mode.
Several parameters affect the decision in what is best practice.
Among them are machine robustness, spindle power, cutter geometry, chip removal, stock material, ...

Rarely the milling modes are mixed for the same type of cutting.
Rough cutting and finishing may use different modes depending the material and the required or reached surface finish.

Lasers, plasma or water cutters for example do not engage with the material.
Still, reversal of the cutting path can have adverse effects.
For example excessive scorching for laser and plasma.

Bidirectional cutting is not supported by QCAD/CAM right out the box.
You can created chronological toolpaths in opposed direction swapping the cutting mode.

Regards,
CVH

In the current job, I am cutting a 3/4 inch wide piece of aluminum with a 1 inch shell mill down to size. So there is no climb or conventional.
It's a process that comes up frequently, essentially top milling with a cutter larger than the material. I'll just keep doing this process manually.

Face milling, right ... It was not in the details.

n_spect_r wrote: ↑

Fri Dec 01, 2023 12:09 pm

I'll just keep doing this process manually.

Solved this with a narrow, elongated but circular closed toolpath.
Adding semi circles or even somewhat larger circles and rounding at reversal point keeps feedrates up.
Even used a very flat ellipse style toolpath so that every axis is always in a certain smooth motion.
Although the toolpath is longer than dead stop and reverse, with a steady feedrate the fabrication time is shorter.
And ... The overall finish is considerable better.

Not supported by QCAD/CAM but you could alter the G-code to go down in Z for the main arc at reversal.
As if spiraling down instead of dead stop, down, continue.
In fact, I use a custom designed G-code macro where the round paths arc radii are related to the requested Feed and maxLinearAcceleration.

Path strategy can be enhanced for gradual engagement, chip thinning, best practice is considering specialized HEM toolpaths.

Regards,
CVH

But even in the example, the tool only descends on one end. I do use this method for milling with a tool that is smaller than the work surface, but there is no need to mill in one direction when the tool takes the whole surface. Thanks for the reply.

n_spect_r wrote: ↑

Sun Dec 03, 2023 12:54 am

But even in the example, the tool only descends on one end.

It was a simplistic representation, a top view.
The arcs are exaggerated, they are calculated from the requested Feed and the maximum linear acceleration.
(My Feed value (mm/min) are usually at least tenfold the reciprocal of yours. )

As is, the toolpath spirals down for the two major curves at both extremities.
(I did mention that this is not supported by QCAD and requires to edit the G-code, simply add Z-nnn to the G2/G3)
The center of reversal is chosen so that the tool is not engaged when 'plunging'.
The first pass starts straight, the last pass is a finishing pass.
The actual center path is identical (drawn very close to distinguish the orientation of the arrows)

Took a while to get the G-code macro perfect.
Feed is dead constant for whole the toolpath from initial plunge to ramp out, beneficial for the surface finish.
Surprisingly, but then not, the fabrication time is shorter while the machine does not exhibit motion jerks.

Another G-code macro is used for a tool that is smaller than the removed area in one way.
As if pocketing and then also using arc's at corners that keeps the feed up. Never plunging down but instead ramp down.
Pocketing is done or conventionally or climbing as it is shoulder milling and not face milling.
I can even pocket out any defined rectangle or square disregarding the mandatory round edge corners of course.
Mostly used to even out an area of a spoil board to clamp things to engrave or whole the spoil board but that may take an hour or two.

The in-build zigzag routine never produced the required fine finish, certainly not at reversals.
Plastics tend to melt, MDF tend to be burned because the Feed almost goes to a dead stop while still engaged.

Yet another macro make a round pocket, spiraling in- or outwards.
Not really a spiral but tangentially connected arcs.

Studied path control in depth and zigzag was mostly a no-go or discouraged.
Initially with QCAD and editing G-code but now the macro's do everything within a few clicks given some parameters.
The macro programmatic language of my EDING CNC controller does not differ a lot from BASIC.
The development time has already paid for itself a hundredfold.

But if it works for you ... Then manually zig and then zag.

Regards,
CVH