PDA

View Full Version : Burnt bit slotting MDF



d4cnc
31-03-2016, 12:57 AM
Hi,
I'm currently cutting some MDF (green -more water resistant) 25mm thickness for a T-slot spoil board. However, I've burnt the 6mm bit I was using (came with the 6040 machine so was more for experimenting).


I've since bought some straight flute bits from toolstation (coming tomorrow) & some 2 flute carbide and 2 flute HSS bits which will take a while to arrive.


I was using the settings on this post for a 6mm cutter.. http://www.mycncuk.com/threads/3500-How-deep-can-i-cut-MDF?p=22357#post22357


(around 800mm/min (300mm ramp/plunge which it ramps down into the slots)


However, having researched more, I realise that they may be a little too slow for my circumstances..


Am I right in thinking that of the 3 different cutters I've ordered, the straight flutes would be good for this job? And that I should be using a much faster feed? Say 3000mm/min at around 6mm DOC (100% diameter)..


How would I know if the machine (chinese 6040) is up to the task? Would the motors stall if it's too fast? Cutter break? Or worse?


Also, for slotting, the toolpath is plunging at an angle like a ramp as it gets deeper towards the DOC. This plunge feed setting by default is around 300mm/min.. should this be upped a lot? This seems slow for the shallow angle it's doing until it gets to depth.


Thanks for any guidance.

JAZZCNC
31-03-2016, 01:40 AM
I've since bought some straight flute bits from toolstation (coming tomorrow) & some 2 flute carbide and 2 flute HSS bits which will take a while to arrive.

Don't waste money on HSS if cutting MDF because they wear out far too quickly.



Am I right in thinking that of the 3 different cutters I've ordered, the straight flutes would be good for this job?

They'll work but you'd be better with spriral up cut because they eject chips better. You'll need good vacuum with straight flute.


How would I know if the machine (chinese 6040) is up to the task? Would the motors stall if it's too fast? Cutter break? Or worse?

If not up too it then could and probably will do both.? The spindle will Bog down and stop cutting causing the steppers to stall, hopefully before cutter snaps. If they don't stall then the cutter will most likely snap.

Shouldn't damage anything on machine really as they won't have power enough to break anything, worst case you'll knock spindle out of tram.



Also, for slotting, the toolpath is plunging at an angle like a ramp as it gets deeper towards the DOC. This plunge feed setting by default is around 300mm/min.. should this be upped a lot? This seems slow for the shallow angle it's doing until it gets to depth.

Yes it's very slow and if shallow angle with multiple passes to DOC then you should be able to cut just little slower than cutting feed.

d4cnc
31-03-2016, 02:12 AM
Thanks for the advice. Really appreciate it.
When you say I'll need good vacuum with a straight flute, do you mean to collect dust or to hold work piece down?
At the moment I've got a just about workable dust shoe around it with a vac sucking everything close to the spindle.. Not great yet version 2 should be coming to fruition soon. As for holding down the workpiece, it has 8 x M6 screws through it holding it to the aluminium underneath.
Also there's an airline blowing air at the minute too but not sure if that's helpful on this task.


Ideally I'd like to get it done tomorrow when the straight cutters arrive if possible but will have a look for some spiral up cutters now too.


On HSMAdvisor, I can't seem to set the straight flute type cutter so am unsure of how to set it correctly. However, when setting it with a 6.35mm 2 fluter HSS cutter at 4mm DOC, It's suggesting 22,000RPM and 2860mm/min feed*. This is suggesting that the power will be 0.62HP (would that be ok for my 0.8W spindle?) and 158% tool life..


Toolstation router bit - http://www.toolstation.com/shop/Power+Tool+Accessories/d80/Router+Bits/sd2579/Router+Bit+Straight+Imperial/p38758


Are these numbers more like what you would suggest?


*2860mm/min is my rapid jog speed - so I assume this is max feed rate I can do. (Seems a little slow but presumably not something I can improve upon without a complete mechanical redesign?)

JAZZCNC
31-03-2016, 03:11 PM
Yes could have worded it better and said dust collection. Sucking or blowing doesn't matter so long has you clear the chips but obviously less messy if can suck.!

Regards the Feeds then First thing I'd say is with these low spec machines then forget what HSM recommends because it's assuming a much stronger machine.
At very best you'll need to drasticly reduce what it recommends, probably 50%.?

I've said this many times and big grevence I have regards these Chinese machines or Low spec Kit machines in that they advertise them for cutting woods and MDF etc when even there Rapid speeds can't reach correct cutting feeds for soft materials. Really pisses me off.!!!

The fact your machine can only rapid at 2860 and low power spindle then I suggest you half the DOC to avoid spindle bogging down and start at half the suggested feed rate then increase using feed override when you see how machine/spindle is handling the load.

Ger21
31-03-2016, 06:00 PM
How much spindle power do you have? I'd start at 3000mm/min and 12,000 rpm, but you can go a lot faster if you have enough power.

d4cnc
31-03-2016, 06:47 PM
Ah I see.. yes, I knew there'd be some hurdles with this machine, but at the price point, it was a perfect choice for me as someone who couldn't even spell CNC let alone know for certain that I'd take to it. I wouldn't have had the confidence to spend much more on what is a very new field. Obviously hindsight thinks otherwise.. ;)

I also bought some straight single flutes.. In HSM it seems to work better..
So having set Feed to 50% (to adjust for lightweight machine), I'm now seeing recommendations for a 6mm DOC of 10k RPM & 1000mm/min. Would this be a good option do you think for initial cutting? (and as recommended.. boost it up on the fly if sounds ok)

Or is single flute the wrong choice for MDF?

*PS.. the plan of getting it done today is out the window..
1/4" router bit shafts in England? Not a good match for the 6mm collet in the machine. New ER11 1/4" coming by Tuesday apparently.




@Ger.. 0.8kW spindle power but just 2860mm/min max rapids..

d4cnc
01-04-2016, 06:39 PM
So a little success.. got the slots cut without issue.. no smoke.. no burnt MDF.. much cleaner cut on the top of the MDF too.. I used 1500mm/min with the 2 degree ramp down at 1000mm/min & then upped it 20% where I could hear a little low frequency vibration.. not certain what it was I didn't go further but I'm happy with the cuts. This was at 6mm DOC & I forgot to mention spindle speed before.. but this was at 12k rpm. Before I was at 18k. Much too fast. So both of these changes probably helped..


The T-slot bit next.. Is the strategy the same? ie. 12k RPM and 1500mm/min.

Boyan Silyavski
01-04-2016, 09:23 PM
Nevertheless between jobs i always clear the bits with acetone and then oil the for conservation. Using a soft piece of towel and carefull not to cut my fingers. The big benefit of straight bits is that they are much cheaper to run, cause they could be sharpened very cheaply and even by you, just passing behind the edge with diamond file. So a micrograin carbide 2 or even better 3 flutes straight bit will always be my preferred bit for wood, laminate, and similar.

d4cnc
02-04-2016, 11:14 PM
Thanks Boyan, I'd not given any thought to bit maintenance, so will go & do some research now.. is acetone recommended for cleaning? I do have some here but would be a bit worried about something so flammable on a router bit..