multiple profile passes without z return or unneeded jogs

[endgrainguy]

This seems so basic, but I can't figure how to quickly program multiple passes on an on-the-line profile, without having unneeded z clearance moves, and return to start point moves before lowering for next cut. I want to go: Z1d, A to B, Z2d, B to A, Z3d A to B, etc. I can do this manually to the code, or program each pass individually alternating climb and conventional feed, but it seems there must be a way to do this quickly automatically (and I need to do a lot of this). I have Aspire V4.5. Thanks!

[Adrian]

Spiral ramps, alternating end points etc are the usual ways. There is no fully automatic way. If your machine has really slow rapid moves then it might be worth the bother but personally I just leave it as it is.

[DLWOODWORKS]

This seems so basic, but I can't figure how to quickly program multiple passes on an on-the-line profile, without having unneeded z clearance moves, and return to start point moves before lowering for next cut. I want to go: Z1d, A to B, Z2d, B to A, Z3d A to B, etc. I can do this manually to the code, or program each pass individually alternating climb and conventional feed, but it seems there must be a way to do this quickly automatically (and I need to do a lot of this). I have Aspire V4.5. Thanks!

Like Adrian says, there's no automatic way to do this. I have jog speeds of 15IPS and when cutting 4x8 sheets of plywood, the unnecessary back and forth can be a bit time consuming, even at 15IPS. It would be interesting to see if this is something the wizkids at Vectric might be able to figure out programmatically.

[martin54]

This seems so basic, but I can't figure how to quickly program multiple passes on an on-the-line profile, without having unneeded z clearance moves, and return to start point moves before lowering for next cut. I want to go: Z1d, A to B, Z2d, B to A, Z3d A to B, etc. I can do this manually to the code, or program each pass individually alternating climb and conventional feed, but it seems there must be a way to do this quickly automatically (and I need to do a lot of this). I have Aspire V4.5. Thanks!

Like Adrian says, there's no automatic way to do this. I have jog speeds of 15IPS and when cutting 4x8 sheets of plywood, the unnecessary back and forth can be a bit time consuming, even at 15IPS. It would be interesting to see if this is something the wizkids at Vectric might be able to figure out programmatically.

DLWOODWORKS Have you tried using spiral ramps? you would have to tweak the bit settings for it to work like altering the DOC & increasing the plunge rate

The toolpath generation in Vectric softwarecould be made more efficient, high end production software has options for things like this but then it costs 20x more

[TReischl]

You can also do it by increasing the slot width a tiny amount. I usually use .002, not sure if .001 works. After doing that program a profile toolpath inside the vectors. You can use spiral or regular.

Of course if your slot has to be exactly .25, precisely, perfectly, this will not work with a bit that cuts precisely .25.

But most things are not that fussy and usually some clearance is required anyway.

[Mark]

Hello endgrainguy,

I am afraid that you cannot really do this with a profile (on) toolpath as it would not be respecting the direction of cut,
but you could instead use the fluting toolpath on the vector, setting the flute type to "Ramp at Start" and the Ramp Length to 0.0.

Cheers,

Mark

[scottp55]

Hmmm:)
Going to have to do an aircut now to get that idea burnt into my brain.
Had never thought about that Mark.
Have to check it out now.
Thanks!
scott

[endgrainguy]

Thanks Mark, that fluting trick works perfectly , giving me exactly what I want with as little work as could be imagined! Saves me tedious manual editing! And I guess this wasn't so basic a question after all. This solution wasn't exactly intuitive, and the other suggestions really were no improvement at all, at least in my situation with my machine. Thanks so much!

[rscrawford]

I'm pretty sure if you profile cut on the line and select 'spiral ramp' it will cut back and forth just like the fluting tool path. I just did that on accident while cutting tonight (didn't mean to select spiral ramp, but it turned out well).

[highpockets]

Great tip Mark, thank you.

Fluting works as advertised, but Vector Profile on line with spiral ramp almost works It cuts back and forth 3 times then rapid moves to start then repeats (Strange).

[Tailmaker]

If you duplicate your vector, reverse one of the two and join to make it a closed vector (even if the return path is on top of the forward path), then you can run "on" this vector with spiral ramps creating a zigzag downward tool path.
Aspire/Vcarve does not care for such tool paths that vectors are repeating over themselves.
However, make sure to set the plunge rate equal to the horizontal feed rate or it may become a bit slow.
One disadvantage is that the machining depth changes over the length of the vector so I am not sure it will really do the trick of accelerating the process.

BackAndForth.crv

(24.5 KiB) Downloaded 100 times