Does anyone else get chatter when doing a straight down drill? I’ve been meaning to ask this for a while, but most of my projects use 1/4" holes, and doing helical drilling doesn’t cause any issues. When ever I just want a 1/8" hole though, It seems it will do the first step down or so, and then get some chatter. Best case I chew up the wood. Worse case, I’ve broken a couple end mills. Seems odd to me it would break the end mills considering the DW660 is meant to be used by hand, and not a a rigid frame. I haven’t tried telling Estlcam to do one continuous drill down, rather than doing it in increments, but also figured I should ask before trying that, so I don’t do something that could damage my machine.
I had this problem with downcut bits, because it wouldn’t evacuate the chips. I either use a single flute upcut, or just drill the first 2mm and finish later on the drill press.
I had this problem with downcut bits
It’s an up cut bit.
just drill the first 2mm and finish later on the drill press.
That’s what I had been doing too. Haven’t drilled a 1/8" hole in a while, and completely forgot it was an issue until last night.
Use a drill bit instead of an end mill.
I’m not setup for doing tool changes yet. Slowly getting there.
Endmill vs. drill bit will make a huge difference. Drill bits are meant to slip on the sides and stabilize the bit as it cuts only on the end. Endmills will bite on the sides and “roll” around the inside of the hole.
1 Like
Endmills will bite on the sides and “roll” around the inside of the hole.
Do you think it would make a difference if I did the drill all in one plunge instead of how estlcam is doing it by going in and out in steps based on the tool Z depth?
I just noticed I already have a “Drill” tool setup in Estlcam with a longer Z step. I can’t remember if I have already experimented with this or not though. This is the problem with getting interrupted by life and work when trying to learn a new thing.
I would expect that to perform worse. Pecking should always work as well, or better than a straight plunge - unless you are cutting into material that can work-harden (like stainless steel) and you are not being aggressive enough with the pecks (which I doubt to be the case here, I recall you mentioning it was into wood).
What kind of end mill are you using? Single flute or two flute? Do you know whether the bit is center-cutting or not? If not a center cutting bit, that could definitely be your issue.
What is your Z feedrate set to when drilling? If too high, this could cause binding and the results you’re reporting.
This is the approach I’m taking - spot drill with the CNC, then finish drill the holes on a drill press later. (But this is on aluminum, I would expect wood to drill reasonably as long as the bit is center cutting and you aren’t plunging too quickly).
1 Like
What do you mean by your machine isn’t setup for tool changes?
Create two separate gcode files. One for the end mill. One for the drill.
That way you can shut off the machine and reset everything to x0y0z0 after you change bits.
Run the first gcode (let’s say, drill steps). Then turn everything off. Change the bits, and then put the end mill back to 0,0,0 and start the second gcode.
I’ll typically use a sharpie or pen to put a dot where I want 0,0 to be
1 Like
I would expect that to perform worse. Pecking should always work as well, or better than a straight plunge
The issue happens when the endmill is reentering the hole though, as if it is catching on the sides when reinserted. If it’s never removed, it wouldn’t catch on the edge.
What kind of end mill are you using? Single flute or two flute?
Double flute.
Do you know whether the bit is center-cutting or not? If not a center cutting bit, that could definitely be your issue.
As far as I can tell it’s good for center cutting. It doesn’t have any problem plunging as it moves down in layers for pocketing.
What is your Z feedrate set to when drilling? If too high, this could cause binding and the results you’re reporting.
3mm/s
What do you mean by your machine isn’t setup for tool changes?
Meaning, I don’t have a way to accurately reset to 0,0,0 after changing out the tool. I have hard stops I can put in to find home on the X and Y, but for Z I have to just move the butting bit to the surface the best I can. For drilling the setup might work, but I’m not 100% confident in the setup for X and Y yet either.
That would seem to indicate that when your router goes up, it’s not coming back down in exactly the same spot. I can think of two reasons that would be the case:
- When it’s first drilling down there is enough pressure on the bit to flex the tool mount so that it’s no longer at the original XY position… (So basically error in XY attributable to Z/Tool flex)
- Or XY position is not being held during the drill process… (So error due to actual movement in XY)
If the cutter is given enough time to cut, there shouldn’t be much pressure on the bit…
This may sound like a dumb question, but are you certain both of your X and Y motors are being driven? When I was rewiring mine recently I had a mistake where my ‘far end’ motors weren’t actually being driven - it wasn’t obvious because their end of the X/Y rods were being happily carried along with the other end, but they would lag by a few centimeters… I had to remove all my belts to verify that they in-fact were not being driven (like I said, really not obvious they weren’t).
I use 2mm/s F(z) with a drill bit in aluminum, and 0.5mm/s when spotting with a single-flute cutter in aluminum. When testing, I’m pretty sure I was using 3mm/s with a 2flute mill in wood (both oak and pine) so I would think 3mm/s should be fine. Maybe try slowing that down so see if it reduces the load on the cutter enough to reduce flex? (although that isn’t feeling like your problem to me…)
1 Like
Often a non-center-cutting mill will work ok for plunging a very small distance - but fail miserably once you exceed that distance. From your other comments though, that doesn’t sound like your issue right now…
I totally get that - I was in that position until about a week ago. I finally broke down and went with the dual endstop configuration with auto-squaring. That plus a Z-probe and I’m now confident on re-finding my work zero, even after a complete power down. A worthwhile upgrade to consider (IMHO).
This may sound like a dumb question, but are you certain both of your X and Y motors are being driven?
I did have that issue, because the pulley on the rear motor had come loose and was slipping, but the drilling issue persists even after I disassembled everything, double checked it all, and put it all back together.
I was in that position until about a week ago. I finally broke down and went with the dual endstop configuration with auto-squaring.
I use my MPCNC as a 3D printer as well, and would have to reflash firmware to switch between printing and CNC to use the dual endstops, and also maintain 3D printing ability. My stops to zero X and Y are probably sufficient, but I do need to get a Z-probe of some sort setup.
Now that I think about it… I honestly can’t recall if the last thing I drilled and had issues was before or after I disassembled the machine and checked everything. I disassembled it after I noticed 3D prints were getting skewed, but I don’t recall if I was working on the prints before or after I was doing some cutting now.
You cab do tool changes without dual endstops. As a piece of evidence, the MPCNC was several years old before we got dual endstops. The some old guy coding video was before we had DE.
What I would do is run one job, when it finishes, return to 0,0,5 or so. The jog the Z up so you van change the bit. Then bring the bit down so it’s just touching and send G92 X0 Y0 Z0. You just need to make sure you aren’t turning off the steppers with a M84 after the first job and be quick enough they don’t time out (or change the timeout).
No new setup or tools needed.
I think a single flute would make a significant difference compared to two-flute. The cutting force deflects the tool and this deflection can cause it to bite as a result of the lateral force, which in turn creates a larger cutting force, causing it to bite still more. Positive feedback can run away.
A single flute is less likely for cutting force on one edge to induce a cutting action on another edge due to the lateral cutting forces.