Official Luthiers Forum!

Good afternoon gents,

I finally have my machine up and working, and just ran my first bit of g-code. What I got was a smoking hole..

I'm trying to make some toe clamps from remnant birch plywood that I have, so that I can use them to hold my aluminum t-slot table slats while I use the cnc to drill and countersink the holes to attach them to my machine. The first thing I'm trying to do is drill two 1/4" holes through my work piece, and into the spoil board so that I can use them as index pins.

I'm having to use Inventor and HSM Express until my copy of Rhino arrives next week, and this is what I have the settings at the first time:

Cutter: 1/4" 2 flute drill mill
Spindle @ 6000 RPM (which is my minimum)
75 IPM plunge feedrate
.0625" pecking depth
.005 chip break distance
No dwell

It worked, but burnt the daylights out of the hole.. I posted up on CNCzone.com, and Ger replied saying use a drill bit, and double the feed rate.

So I then used a 1/4" brad tip drill bit that I have at these settings:
Cutter: 1/4" Brad Tip drillbit
Spindle @ 6000 RPM (which is my minimum)
150 IPM plunge feedrate
.0625" pecking depth
.005 chip break distance
No dwell

Still smoked..

Any ideas?

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

Jason look at the problem, analyse it, then make your changes! Problem is, the wood is burning, and that means it got too hot using your current settings!

I personally think your .0625 peck depth is too shallow for wood, as this causes the bit to engage the hole multiple times, though you did not give the thickness of the material.

Assuming it is .750" thick, if I were doing it I would peck at least .150" deep at about the 150 ipm mark! I think you will see a difference. I would also do a two stage drill procedure. I would drill undersized about .020" for the first step then drill to size for the second, and keep in mind if you are using a router instead of a spindle, you will have run out and you need to compensate for that as well. Take a scrap piece of the wood and do the drilling procedure in the scrap, measure the final hole and if necessary buy an undersized bit to use for your final drilling step. If not, standard size index pins will drop in the hole and not give you a true position.

Mike

I agree that the peck and chip break distance is way too low. Here's a video of me drilling 3/16" holes into EIR with hard maple plywood underneath. I didn't bother with a chip break in this case. Feed was 75ipm, speed about 5000rpm (although I think I recall having to up the speed a bit because it stalled at 5000).

For 3/4" plywood, you should be able to drill through it in one pass. You're burning because your bit is in there not cutting way too long.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

yeah, fwiw, i think the pecking is the problem. the tool isn't engaged enough and you are burnishing. also no point pecking with a brad point because the point guides the drill. when you retract, the tool losses some of the centralizing feature that is the whole point of that type of tool.

Video didn't show up for some reason

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Guys,

Thanks for the responses. I can't wait to get back out there, and try new feed rates. Andy, after seeing that video, I think I may give it a shot without the pecking. Looks like it drills through wood like a hot knife through butter. I'm going to try and get out there tonight, I'll update my post when I do. ONE of the issues is that I was told my z axis ballscrew was a 1610, when its actually a 1605. So it was not only traveling only have the distance it was supposed to, but also at half the speed.. So if I was using 75ipm, it was actually traveling at 37.5ipm.. It is set properly now, so 150ipm should be 150ipm.

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

Ok, here we go! So, I was so psyched up to be cutting something with the proper settings, that I completely forgot to change the drill from peck to straight drill. I changed it in the gcode that I used to drill the spoil board though, and it did seem to cut better. One thing that I need to fix before I do anything else though, is how flexible my temp table top is. It was probably deflecting a good 1/4" or more. I'm hoping that a layer of 3/4" MDF on top of what I have now, screwed down will be enough. Any suggestions?

Video:

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

My rule of thumb on pecking in wood is 4x diameter.

You need to feed at a rate that provides the correct chip load.
Your chip load for a .25" bit should be in the neighborhood of .01" per tooth and at 6000 rpm that puts the feed rate at 120IPM

In practice, I've found drilling at SFM speeds of 25%-30% of wood's 2000sfm rating works best so you could increase your rpm to 7500 and use your feed rate of 150.

3/4" MDF has made a good base for me both when screwed to T-Nuts in my slotted table