[iainlines]

Hi all,
I operate an AXYZ 6010 twin head machine with 5hp ELTE spindles. I am quoting on sub contract work to cut 1" thick moisture resistant MDF. I'm just after some feed rates stepdown advice if anyone can.
My customer seems to think they cut in one hit with a 12mm cutter
Thanks
iain

[ger21]

I'd try it in one pass with a 12mm (1/2") 2 flute compression at 16,000 rpm and 400ipm. If your spindle is up to it, you can probably go up to 500ipm.

[iainlines]

As fast as that? I spend 90% of my time machining foam but also do some mdf and ply. Our machine sellers recommended 4metres/min (around 160 ipm) for 12mm thick board. I'm not saying you are wrong as I am very new to this but 400ipm, or 10 metres/min sounds very fast. The spindles are only 5hp, will they stand up to that?
Thanks
Iain

[ger21]

If you had a 10HP spindle, then I'd recommend a 3 flute at 20m/min.
I don't know how rigid your machine is, or what your spindles can handle. I'd program it for 10m/min, and start cutting at 50% FRO and dial up to see if it can handle it.
The faster you go, the longer your bits will last.
If you find you can't go that fast, then I'd try two passes, as fast as possible.

[KCSF_DUST_MAKER]

I run a Biesse Rover 346 and a Weeke BHP-008 in a production shop and cut 3/4 MDF, melamine, osb, furniture grade ply and laminates regularly. My fave bit/feed/rpm combo on the Rover in 3/4" mdf is a 2 flute 1/2" compression bit, spun at 18,000 and fed at 18 meters/m. On the Weeke I have other tools to pick from and use a 3 flute 3/8 chip-break style bit on things that are going to be sanded anyway. I spin it at 20,000 and feed at 20 meters/m. For things needing a more finshed edge I use a 1/2" 2 flute 3deg down shear spun at 18,000 and fed at 15 meters/min. I would use a compression bit here but being a flatbed machine, ive had trouble with compression bits picking up parts and breaking the vacuum. Ive been begging for a 1/2" 2 or 3 flute down spiral to do this with but the powers that be think that chipbreak cuts just fine. The age old argument between operator and management.

[mmoe]

If you had a 10HP spindle, then I'd recommend a 3 flute at 20m/min.
I don't know how rigid your machine is, or what your spindles can handle. I'd program it for 10m/min, and start cutting at 50% FRO and dial up to see if it can handle it.
The faster you go, the longer your bits will last.
If you find you can't go that fast, then I'd try two passes, as fast as possible.

The one downside to two passes is that it wears only the bottom half of the bit down because the top half never engages the material. It's kinda 6 to one, half dozen to the other whether you go faster with a half depth pass or go slower (wearing the bit down a little) on a full depth pass. Neither is ideal and both will have adverse wear to the bit.

[mmoe]

I run a Biesse Rover 346 and a Weeke BHP-008 in a production shop and cut 3/4 MDF, melamine, osb, furniture grade ply and laminates regularly. My fave bit/feed/rpm combo on the Rover in 3/4" mdf is a 2 flute 1/2" compression bit, spun at 18,000 and fed at 18 meters/m. On the Weeke I have other tools to pick from and use a 3 flute 3/8 chip-break style bit on things that are going to be sanded anyway. I spin it at 20,000 and feed at 20 meters/m. For things needing a more finshed edge I use a 1/2" 2 flute 3deg down shear spun at 18,000 and fed at 15 meters/min. I would use a compression bit here but being a flatbed machine, ive had trouble with compression bits picking up parts and breaking the vacuum. Ive been begging for a 1/2" 2 or 3 flute down spiral to do this with but the powers that be think that chipbreak cuts just fine. The age old argument between operator and management.

A good compromise when you aren't getting good vacuum holddown is a mortising compression bit, which has only the bottom 1/4 inch of upsheer. This creates a downspiral type balance of forces since most of the cutting edge is downward, but still has the upsheer at the bottom to keep it clean.

[mmoe]

As fast as that? I spend 90% of my time machining foam but also do some mdf and ply. Our machine sellers recommended 4metres/min (around 160 ipm) for 12mm thick board. I'm not saying you are wrong as I am very new to this but 400ipm, or 10 metres/min sounds very fast. The spindles are only 5hp, will they stand up to that?
Thanks
Iain

Gerry is correct. 400ipm would be on the slow end of the spectrum for some machines. 160ipm for 1/2 inch plywood is crazy slow. You're just going to wear your tools out at that feedrate. If you think about it, if you have a 2 flute cutter at 15,000 rpms and travel 160 inches per minute, you're only removing .005" per cut (160 divided by 32,000 cuts). Most 1/2" 2 or 3 flute cutters are capable of taking a .015 cut without much stress at all, so that means they can operate at 3 times your 160 IPM feedrate, or 480 IPM. If you have a 3 or 4 flute bit, you may get even double that without much trouble. Obviously, that .015 cut is over a slightly larger surface area than the bit width (since it is really half the circumference) and the height is double a 1/2 inch board as well, but a genuine 5hp spindle (not some small hand router in a clamp) shouldn't really have much trouble making that cut. Also, MDF cuts like a hot knife through butter.

Not knowing your machine, I'd also start out at perhaps 200ipm, and increase until it seems to be cutting in the sweetspot where there are solid chips (instead of powder) and the finish on the edge is still good. I suspect you'll get to 400ipm no problem. You'll also get less heat running those speeds, so less chance of getting that burned edge to the MDF.