What went wrong

[monlover]

Hi,
this is so bad and i relly need help to understand what went wrong hear,
cutting a project with 530 holes, hole diameter is .285 and my down cut bit is .22 so I tried to use drilling toolpath option but did not work
so i picked pocket toolpath option, all was good until i smelled some smoke and the spoilbord was aught in fire.
please take a look at the tool setup and tell me what was wrong on the setup, is it the plunge rate? or the speed of the spindle?
after sercheing online about plunge rate, they said plunge rate has to me less than 50% of feed rate. But how to find out the correct feed rate for drilling MDF or any other material.
is there any chart can show feed and plunge based on bit diameter and which material can be used with??
Thank you in advance.

[gkas]

NEVER use a downcut bit to drill holes. The sawdust is packed into the hole. It will burn even shallow holes. Use a special CNC drill bit, an upcut bit, or a straight bit.

[monlover]

Thank you for the reply, what speed, feed rate and Plunge rate do use?
Thx

[ger21]

Don't use a pocket toolpath, use a Profile toolpath inside the vector, and use a spiral ramp. Ideally, you don't ever want to plunge.
My belief is that with wood, you can always ramp (or even plunge) at full speed. Going slower only causes burning.
As for feedrates, go as fast as you can, while maintaining the desired quality. This may be dictated by your machines ability. The faster you go, the longer your tools will last. Only slow down to increase quality.

[TReischl]

You told the tool to plunge up to .75 all at once at 100 inches per minute. Essentially you were using a downcut bit as a drill.

The advice above about not using pocketing to drill holes is correct. Profiling with a spiral ramp is the way to go.

[TReischl]

You told the tool to plunge up to .75 all at once at 100 inches per minute. Essentially you were using a downcut bit as a drill.

The advice above about not using pocketing to drill holes is correct. Profiling with a spiral ramp is the way to go.

[scottp55]

IF you'd been using a full vac hold down with plenum and DC you might very well have had 2 separate fires and lost the shop

I'm only showing this to elucidate on Gerry's advice.
Every machines OS and abilities will determine the exact X,Y Feed on small holes(and different speeds for different diameter holes usually).
After you chuck a suitable bit, I would Highly recommend clamping some scrap MDF and do some test cuts a hole at a time half depth,
and feel the bit after each hole until until you have Feed and Plunge set so that bit is room temp after the hole cut...Then do full depth test....
Then multiple hole test full depth.
I had to do 3 off these with 2 diameter holes, and there were 600+ holes full depth each...and I had to use Plunge rates that were spooky to me at the time to keep bit cool. Took maybe 10 single hole/half depth tests to get Plunge right...and then some more tweaking to get 10 holes full depth with a cool bit.

Plunge rate and RPM is more effective to control bit temp, than Feed on small holes that are spiral ramped....also note the number of ramps I wound up with.
And then I made 2 more within months...and after all 600+ holes were done....bit was cool to the touch:)

THIS IS ONLY FOR MY MACHINE!
The bit I bought for my holes was on recommendations from someone I trust....Many bits are suitable, but single flute O's are more in keeping with my 1hp spindle.

One you've got the bit tweaked...maybe add a DRILL ONLY (Actually a Ramped Profile cut) category as the Feeds and Speeds are SO different?

This is ONLY an example so you can slow preview, and look at that toolpath which works so well!
Be sure and measure holes after test cuts, so you can Tweak Offset for an EXACT size hole if needed....for my threaded inserts, I tweaked offset 4 times..
And dowels 3 times.

MAY be a good starting point for ONE hole....test, Test,TEST!!!
Normal clause for absolutely NO responsibility for ANY results are applicable!!

ZZZ EXAMPLE ONLY RAMPED PROFILE.crv

(218.5 KiB) Downloaded 54 times

Be careful!
scott