im considering adding drill on one of my cnc plasma machine and i dont want to use z axis to have the force on the drill as it might snap the bit so im considering using http://cgi.ebay.com/DESOUTTER-AFD22-AUTOMATIC-AIR-FEED-DRILL-NEW_W0QQitemZ110412824219QQcmdZViewItemQQptZLH_DefaultDomain_0?hash=item19b51dfe9b&_trksid=p3286.c0.m14

or someone have a better suggestion? or is z axis with pecking option is the best route?

im open to ideas

Cheers
Dan

Dan,
That looks like a good idea. I saw another air drill on ebay recently. I went looking for it but couldn't find it. Check out the link here:

http://victoryplasma.com/victorycnc/currentimages/

I am not sure if those are "real" pics. I think you would have to drill before you cut or clamp and re align. Their drill head looks like an air system.

How did your oxy/fuel project go?

WSS

the oxy n fuel project is waiting for parts that i order over 2 months ago for my machine torch so im pretty stuck on that one.. (i was expecting to drill everything first before starting any cutting (that option would be nice for some parts that requires tapping or small and senstive size holes

set up you feed rate on the z axis proportional to drill speed if you have it set properly you will not break the bits.start with .oo3 per revolution smaller drill bits have to run fast to keep from breaking. multiply3x cutting speed required 80 is a good speed for HSS in cold rolled steel diviced by the diameter of the bit.

what type of drill do you suggest me to run?

vfd spindle?

you will need a varable speed spindle to do any kind of serious drilling in metals.What is the desired purpose of the drill you are placing on the machine, drill holes in aluminun,steel...? what size drills do you want to drill? I have seen the drilling head from a milwaukie mag base drill press mounted on the gantry. It depends on what you intend to use the drill for in the first place. The air spindle you linked to looks like it may work....just thought I would pose some questiions for thought.

for me i think i would be drilling 1/4 holes in 3/8 thick material that way i can use that material for tapping after

if i do get that vfd spindle i could use it for my cnc router too compared to the current porta power router i have (friggin loud)

maybe ill actually even run rotabroach on that cnc too like that victor table..

what kind of drill is on that victor table? looks pretty nice setup

Dan,
I couldn't tell what type it was. Question on the rota-broach- Is that an annular cutter that spits out a plug when your done? That would be awesome to be able to drill in that manner. I drill 11/16" holes (W/a annular,mill mounted) in 1" A36 a whole bunch and it would be cool if I could do that on my table before cutting. I think a dedicated drill head would work best. I think you can do your drawing by layer to off-set the operation/action. I have yet to operate a CNC machine! Sometime in the near future I hope.

Good luck, I will keep my on your progress.

rldmachine, I will copy your info you listed about drill feeds/speeds and keep it handy. Thanks!

Cheers!
WSS

rotabroach is another term for annular cutter (they have 3 different terms i forgot the last one)

for running multi operation it would be very simple to do wtih sheetcam

having different relay to turn specific stuff on and off and the tool offset

once im "ready for tool change" i can drop the torch lower than the drill and start cutting after all drilling is done

for my big machine (5x10) is the machine i plan to add drill head on it has cutting torch/plasma and hopefully soon ill have drilling head on it

There are a couple of ways to get there. You can mount a separate Z mechanism on the same carriage as your plasma head and let it have it's own motor and driver (independent Z2). At that point you have total control of both processes provided:

1. Your Z is a real axis and part of the toolpath
2. You can change the POST in the CAM to work with two Z's
3. Your hardware and control software can support the additional axis.

We helped program a machine recently that had to do mixed processes (drill, route and plasma cut. It even had to be able to mount two router motors and use a different tool in each, all on the same table. It ended up being a 4 axis (5 motor/5 driver) setup with there being X (dual drive), Y , Z1 and Z2. Either Z could be: plasma, spindle (high speed) or special process (marker, center punch, drill)

For the average hobby guy or small shop building a plasma table I don't advocate a mixed use table unless they don't have the physical space for two tables and they don't mind spending the time to switch over the physical setup. For a shop that builds a custom product or needs the flexibility of doing multiple processes on one machine that saves handling and labor, the multi-use machine starts to make sense.

Because the plasma control (with DTHC) through MACH3 uses a normal Z axis (even for THC control) switching to another process on that or another axis is a 10 second software profile change. By writing a custom POST in SheetCAM, the tool number automatically determines the active axis, retracts the non-active axis, AND applies an automatic offset so it does not have to be done manually in the CAM program. It will switch back and forth between the heads and position them properly based entirely on which tool number you select in SheetCAM. Since the feedrate and even the process (peck drilling, etc) are a function of the tool definition, all of that is automatic too. It does it by switching the Axis call (turns what would be Z moves in the g-code to "B" axis moves and apply a fixed XY (and B if needed) offset for just that process.

On a table designed to do 2 axis of motion and there is no true Z (only a torch lifter and independant ATHC) your options start to diminish. Most often it is not as simple as just adding another axis (slide and motor) because the software does not support the new axis. You can, of course, make it totally manual and just build something to do the one process you want and trigger it externally, but things like offset, feedrate, spindle RPM and peck cycles will be difficult to impossible to do.


Tom Caudle
www.CandCNC.com