How to profile cut an open vector

[cloudcabinarts]

I've got a chair leg I'm trying to cut out of 1" cedar. One long edge will not be cut and I will use hold down clamps on this edge. I've imported the drawing into Vcarve and have deleted the edge I don't want to cut. I can't figure out how to get it to run the cut length at .25, reverse and come back the other way at .5, and again at .75 and 1" without going back to origin each time. I'm sure this can't be that difficult but I'm stumped.

[WaltS]

You can cut an open vector with the fluting toolpath. Not sure about going back and forth though. One of the experts will chime in shortly and give you an answer to that.

[Adrian]

Easiest way is to set a Spiral ramp on the toolpath. With the cut depth set to 1" and the pass depth to 0.25" that should do what you want.

EDIT:Scratch that. I misunderstood what you wanted.

[cloudcabinarts]

I'm using the profiling toolpath, using 4 separate toolpaths, one for each pass; first and third conventional, second and fourth climb cut. So far I've got the first pass set as conventional and it goes fine, when it gets to the end it comes back to origin and climb cuts each small segment of the overall cut, taking forever, it's not continuous. I've tried grouping the segments and this doesn't work.

[Adrian]

What do you mean by grouping the segments? Sounds like you've got a whole series open vectors rather than one continuous one. Use the join tools (select two vectors, right click and choose the relevant join from the menu) to make it into one vector.

Climb and conventional doesn't really apply to open vectors as both side of the cutter are in continual contact with the material.

[tomgardiner]

You can do what you want. First, assuming that your leg drawing is with joined vectors, you will have to cut your vectors at the corners to give you individual line sections that you want to follow.
Select Vector to cut. Type 'N' to enter node editor. Hover over node where you want to cut and type 'C'. Do this wherever you want to cut vector. Esc or N to exit node editing.
Use the profile toolpath. Select your vector, outside profile, go into ramp window and select spiral ramp. Calculate and check to see if the profile is on the correct side of the vector. You can enter node edit and change the start point by hovering over the opposite end of vector
from green square. Type P and it will now be the start. Recalculate and you are almost there.
You will want to extend your vectors so that the cut extends beyond the ends of your workpiece. You can do this with Leads window click on lead out. That should do it.
Oops, beaten to the punch.

[cloudcabinarts]

That was exactly it. I tried previously to join all vectors and it didn't work because there was a group in the selection. Ungrouped and joined fine.

Tom G that sounds like what I'm looking for, getting real close, thanks. The spiral ramp is the idea, to take it further I went to Edit passes, clicked to maintain exact tool depth and passes set to one, and it appears it's now doing it in "one" pass, within the limitations of the bit settings, so 3 passes here at .4, .8 and through, back to back and considered one pass by the software. With it set to two passes, it goes three passes, twice. Now the only thing is it's still ramping the entire length and not maintaining exact tool depth. Any thoughts on that.

The leads are new to me and I see the use, apparently they can't be used with a spiral ramp.

[4DThinker]

Not sure if this will help, but when I've got a single connected profile edge that I want to simply go back and forth along the vector rather than pick up and go end to start repeatedly, I make an offset vector 1/2 the diameter of the bit I'll be using outside the actual profile vector. This offset vector doubles back on itself exactly. Now I use a profile toolpath ON the offset vector. If the double-back vector is closed the bit simply steps down one pass depth each time it returns to one end. If open on one end it will return to beginning (always staying inside the cut path) then lift to safe height before plunging down again to continue. Either way this strategy leaves any clamp that might lie between the beginning and end safe from any traveling bit. As the bit is air cutting (inside the previous cut path) when it returns to the beginning the direction it goes when cutting (climb or conventional) will remain the same.

4D

[tomgardiner]

The continuous ramp the length of the toolpath is what the spiral ramp does. I use it for hardwood cutting when I can't put much load on the part. It will ramp down to the depth of the pass then run over the toolpath at a fixed depth so when you call for two passes it will run two ramps then once more at full depth.
I wasn't aware that leads aren't recognized for spiral ramps but you can add leads in your drawing to do the same.
Another strategy to cut profiles in solid is to cut a series of profiles full depth offset from your final profile so that you work your way inwards toward the finished cut. This is something I manually drew with a series of offset vectors joined with lines at the end to create a zigzag cut.

[cloudcabinarts]

Good ideas, thanks all! There's more than one way to skin a cat.

[CosmosK]

I've been doing this recently. I do three passes climb, one conventional and a final climb pass on a hard wood part profile. To get the back and forth, I have made them each their own toolpath. That does pretty well, but there are retracts to z safe between the paths, so I go in the code and edit those out. It's working great. FWIW, I'm finding climb gives me a better finish. Convention tears out material, sometimes even very small. My second to last pass in conventional because the last thin layer of material to get removed can get sucked into the climb cut and leave marks on the profile. I try to leave 1mm for the climb cut then turn around with the finish pass taking 0.3mm. Surfaces are coming out great. 3 flute 5/16 end mill.