Semi-manual Milling

I'm a hobbyist working in a definitely non-production environment, and I'm considering a CNC conversion of a Bridgeport mill. I am comfortable with CNC, since I've built a fairly large CNC router before, and I am familiar with the control setup, mach3, mach 4, etc. I also have plenty of tools to pull it off without it being janky.

My plan is cnc control the X and Y with ball screws, and the knee as my Z axis. I know this won't result in very fast plunge or retract moves, but Again, I am doing low-volume, and mostly need the cnc capacity for handling complex curves and helical hole interpolation.

Anyway, here's the real question: I am accustomed to using Fusion360 + Mach3 for my router, and on my router, I do manual tool changes. I know I can do the same things on the Bridgeport, but, because the bridgeport will be slower, and because my conversion leaves the quill unchanged, I was hoping that I could program in not just tool changes, but manual operations. So, if I have a CNC milling/drilling project, I could program a pre-drill location, have mach3 position the hole and then wait while I drill the hole, then put an end mill in, and then continue with a milling operation. I might also use this for tapping where it positions the XY, then I drill, hit continue, new XY, drill, etc. then the same with taps.

Has anyone else done this? what are the relevant G codes? would I just insert a "blank" tool change, perform the operation, and then a real tool change? could I write some kind of pre-canned routine for essentially going to a location and then doing nothing?

Has anyone ever managed to get Fusion360 to produce code like this?

I run a prototrak mill at work that can be run like that. It is pretty handy if you have a lot of holes on a one off part.

I don't know much about Mach3 controllers but I ass-u-me you could program to position over the hole you want to drill, insert an M00 into your program and drill manually. You may want to call out your tool and safe start line after every M00 so you could start your program at any location.

This is all assuming that you aren't having the spindle on/off controlled by your program.

I have an Acer knee mill with Anilam control that I run like that, works great. I too use it for complex curves and hole location. I pocket mill large holes, but follow up with a boring head if it matters.
I also use F360- i like it


Sent from my iPhone using Tapatalk Pro

as far as hole tapping with a knee driven machine and free spindle, I made the tap the next tool number after the drill and did this:

drill all the holes 1st

standard tool change to put tap in chuck

g0x1y1 (move to hole position)

m3s150 (spindle on, slow enuf to count tap revs)
m00 (machine sits, tap spins, lube and stick tap in hole, count revs for depth, when to depth, hit cycle button)
m4m00 (tap reverses and screws out)

g0x2y2 (move to new position)

repeat next 3 lines as needed.

you could also incorporate all except the move into a subroutine if you have a lot of holes to make it worth it.

easy peasy.

as far as drilling then putting in end mills, yada, do your milling, then your drilling, then your tapping.