Optimise by flipping direction when several passes are required

[newyd_cnc]

Dear all,

QCAD /CAM is a great tool.

An optimisation I see could help increase efficiency considerably would be to allow "flipping" the direction of machining when several passes on the same profile are required.

In the simple example i attach here, the lines are cut at 18mm in three passes. The g-code sends the tool end from A to B extremities of the line at the Z depth of the first path, then travels back to A in the air , before going down at the second Z depth and cutting A to B again, ...

Now, I am sure this behavior must have been object of discussion in the past, however I only saw it mentioned once in the forum when pocketing capabilities were being discussed.

I was wondering, how far is QCAD/CAM potentially from the ability to reverse path direction (flip) on several passes on the same profile? I believe the optimisation and time economy would be significant.

Thank you

[CVH]

The issue here is that you decide somehow on the method of milling, Climb vs Conventional cutting.
Based on the method that is best suited for the project at hand depending the mill type, material type, stiffness of your setup and so on.
Other criteria are: Cleanness of cut, available power, chip removal, re-cutting of chips ....
... Side-milling, face-milling, deep groove milling, ....

It is OR Climb cutting OR Conventional cutting.
If you travel back in reversed on the same route while engaged with the material then you are mixing the two milling strategies.

In the end it really won't matter a lot.
Rapid (air) moves are done at the highest achievable Feed (G0).
While milling may be done at less than 1/10 or even 1/100 of that Feed.
And there are other benefits like for example alternated loaded operation of your milling motor.
About none is constructed for 100% usage at full load.

The only minor disadvantage is the total traveled distance.
But then again, the average Feed increases.
There is more to be gained by an optimal cutting Feed for a given tool and the used strategy.

Regards,
CVH

BTW: See Private Messages.

[newyd_cnc]

Thank you for your feedback CVH, it is much appreciated. I understand from your answer (although it is not staed explicitly) that a function like I described is not available in QCAD/CAM?

I understand our explication but in my case I am CNC cutting large softwood panels, rather than small block of metal (aluminium, steel or other) and I am not sure the points you raise are entirely fitting to my situation.
When I program to cut a 2500mm long line (as in the example I posted) in OSB wood, having the machine retrace back the 2.5m at the end of each pass to start a new one, even at high feed it "feels" less than optimal in terms of time.

I am sorry if what i imply here is a NO-NO ! in CNC cutting however, I think that in the case of soft materials with localised vacuum chip removing, it could be interesting to flip the direction of passes over identical profiles.
Regards
LB

[CVH]

Yes, perhaps true but not entirely, it is called a profile for something.

This comes from Profile-milling or Side-milling.
Mostly reducing stock material to some defined external profile and/or enlarging voids to an inner profile.
The initial inner cut is Slot-milling and kept to a bare minimum because the cutter is engaged for 100%.
That won't be neat and not precise, best practice is usually not more than 30% and even less for finishing.
Also meaning that for creating a profile like a 'slot' we use a cutter of less to about half the width of the slot.

On the other hand ...
We all know that even with Groove or Slot-milling and even in soft materials there is a neat edge and a lesser neat edge.
When routing out pieces from board material it is the idea to have the neat edge at your required piece side and the lesser neat at the spoil side.
For most of the less costly or less stable aka rigid setups that would correlate with the Conventional milling side.
About all flat bed routers belong in the category 'Not rock-solid' ... Very high stiffness is simply not achievable.
The larger the spans, the more it can flex.

And even then it relates greatly to the used cutter and other criteria.
Most beginning or DIY machinists consider anything sharp that cuts as it spins as being a milling cutter.
But there are a wide variety of very specific cutters, contact your supplier for advice on best suited.
Not all end-mills are for example capable/intended of/for diving into material from above.
BTW: Here I would advice a down-cut cutter there it doesn't tend to lift your material up.


And no, there are but 2 trajectory controls implemented in QCAD/CAM.
One can indeed adapt the QCAD/CAM profile output fairly good to be usable for Water, Laser or Plasma cutting.
And one can also exploit it for Slot-milling or (Deep) Groove-milling with the obvious draw-backs.
Although that many of the applications would have contours with a closed nature.
The major hurdle I see is supporting G41/42 and reversing the cutting direction.


The biggest issues here are probably the limitations of your router.
For routing in wood with for example a 6mm carbide cutter at a typical surface cutting speed of 460 MSM the typical SPEED is about 24000rpm.
With 2 flutes and an average chipload of 0.3 mm per tooth the ideal FEED would then be 14400mm/min.
(For imperial users: 1/4" cutter & 1500SFM; SPEED≈23000rpm; 2flutes & 0.0125IPT; FEED≈575IPM ... 14600mm/min)
Remark here that the used values are for a tool life of about 1 hour and a cutting depth of 1/2D to 1D.
Tool life (In hours) increases with reducing the rpm ... For sure, but it takes longer to fabricate the same piece

If it is really intended for wood then your setup would be capable of that and maxFEED should at least be 2-300%.
Meaning that it would take about 10 seconds to do the 2.5m long cut and 3-5 seconds to traverse back.
The reality will be far less.

Using a 6mm cutter on a 2.5m board can relatively be considered as micro-milling (>100:1) what requires:
High FEED, high SPEED, moderated depths and less cutting power.
With a 8mm cutter at 3 times the diameter deep it would already be acceptable to cut a 22mm thick plate in one pass.
The only difference is that you remove about 33% more material.
But it can be done in less production time.
Bottom line: You can't have it both ways or you need to upgrade (See below).

A work around for cutting a board up in the length or traversed might be G-Code macro's.

More practical:
Increase the RPM of your milling motor from min to max just above the material and somewhere halfway.
There will be 2-3 regions with minimal vibration, one can verify that by touch or with a measuring device.
Make some trial cuts around those SPEED's and various FEED's, there will be an audible sweet spot and that will deliver a most perfect cut.
Increase depth per pass until it it obvious that the rpm decreases, the cut get worse or the tool breaks, use 70-80% of that.
Have a closer look at your chips ... When it is rather dust then you are re-cutting them ... Decrease SPEED and/or increase FEED.
Also inspect your side finish, when discolored or even burned then your SPEED is to high and/or your FEED to low ...
... Or the tool starts to become blunt.

Regards,
CVH