Multiple passes in the x-y plane rather than z

[dirktheeng]

All,

I'm interested in milling 5 piece, raised panel doors for cabinets. I have worked out all the jigs needed to hold the pieces and am now working on the cam solutions. I saw that vectric now has the ability to put a profile on the outside of a piece via a profile bit (sucha s a roman ogee). The software seems to be stepping the passes in the Z direction. This will work fine for any profile bit that has no undercut to it. If there is an undercut, you have to approach the stepping from the x-y plane, not the z direction. I can create my own tool paths via Inventor (or other CAD), but that is a decent amount of work. It would be much easier if the CAM software would give me the option to step this way rather than in the Z. I wanted to ask about this b/4 I put in the work to generate my own tool paths. Let me know if anybody has an easy solution. My motto is KISS (Keep It Stimple Stupid) so taking the path of least resistance is always good.

[Mark]

Hello Dirk,

You can add a lead-in / lead-out (Profile toolpath > Leads tab) to allow a tool to approach a profile cut
from the side.

I hope that this helps.


Cheers,

Mark.

[dirktheeng]

I am aware of lead in/outs. They can help ensure you get a smooth approach to your pass so the tool doesn't sit there generating heat. However, that is much different than stepping your cuts. You step your cuts to make sure you don't take too much material off in a single pass. This is especially important in milling end grains. You will have to step your cut to mill a pannel well. I do need to step in the x-y plane rather than in the z direction.

[tmerrill]

The only approach I can think of would be to create multiple profile toolpaths and 'walk' the bit in using a decreasing Allowance Offset.

It's not as hard as it sounds.

Create your first toolpath with the largest Allowance Offset you need and set the lead-in, lead-out. BE SURE to edit your tool and set it's pass depth to whatever cut depth you need so it is a single pass toolpath.

Now use the Copy Toolpath icon to create a copy. Double click on this to edit it, change the Allowance Offset to a smaller value, and recalculate. Everything else will be the same as the first toolpath.

Repeat as many times as you need to.

Now, with the toolpaths in the correct order, check them all and save them to one cut file. Only negative things I can see is there will be a retract and plunge between each pass and I don't think this will work with an open vector, just closed shape.

Tim

Tim

[Mark]

Hello Dirk,

Tim beat me to it

Cheers,

Mark.

[dirktheeng]

Thanks guys! This is much easier than making a tool path by cad. I can easily edit the gcode to take out the z moves if they pose an issue, but they wont unless I go into some fast production... which i won't.