PDA

View Full Version : Chipload and DOC for small endmills



Jonathan
15-01-2011, 04:52 PM
What chipload should I use for a 3 flute 1mm endmill on aluminum, for slotting and for other cut widths.

I've been researching and found anything from 0.005mm to 0.02mm per tooth.

I really don't want to break this so I thought I'd ask here first...

Depth of cut I thought maybe 0.5mm for slotting, that might be a bit much though?

Robin Hewitt
15-01-2011, 07:49 PM
Depends on flute length, spindle speeds and lubricant. What you got?

Jonathan
15-01-2011, 08:02 PM
Depends on flute length, spindle speeds and lubricant. What you got?

Flute length is small, maybe 3mm. I only need to cut down a maximum of 1.4mm though. It's HSS.

Spindle speed, milling machine is 2150rpm...so very limited for this size of cutter. If I bolt the router spindle to the milling machine when I get it that will get 24000rpm - so still less than optimal but much better.

Lubricant would be me standing there with a brush and cutting fluid. Maybe WD40 as it's thinner so should get into the flutes more easily?

M250cnc
15-01-2011, 08:16 PM
If the cutter is a centre cutting type I would chain drill it. As a cutter that small is stronger radially than axially.

You also are not going round re cutting chips.

I would step all the way round 1mm then when you are done step 0.5mm then step 1mm again to cut out the webs.

You have then removed 90% of the waste and can then finish the slot.

For chip load 0.01 per tooth max.

But someone of your experience I thought you would have known this. Lol

Phil

Sent from my HTC Desire using Tapatalk

Jonathan
15-01-2011, 08:28 PM
The slots I'm cutting are 1.4mm wide and 1.3mm deep. (see my Gcode thread and look at timing pulleys program if you want to know exactly what's what...)


As a cutter that small is stronger radially than axially.
I think you meant stronger axially.

I think it's center cutting, not sure ... quite a big change to the code to do that but worth it I guess.

Where do you get the 0.01mm chipload number from, experience (if so good)? It's about the average value I found from checking various websites. I've used 0.025m chipload with 2mm 3 flute endmill successfully:

http://www.youtube.com/watch?v=p13LZ6IxmgY
(wrong title on that video!)

I may just grind a form tool to do this in the end, but it'll be nice to try it.

Experience! Only 7 years...much less than yourself I guess.

M250cnc
15-01-2011, 08:53 PM
The slots I'm cutting are 1.4mm wide and 1.3mm deep. (see my Gcode thread and look at timing pulleys program if you want to know exactly what's what...)


I think you meant stronger axially.

I think it's center cutting, not sure ... quite a big change to the code to do that but worth it I guess.

Where do you get the 0.01mm chipload number from, experience (if so good)? It's about the average value I found from checking various websites. I've used 0.025m chipload with 2mm 3 flute endmill successfully:

http://www.youtube.com/watch?v=p13LZ6IxmgY
(wrong title on that video!)

I may just grind a form tool to do this in the end, but it'll be nice to try it.

Experience! Only 7 years...much less than yourself I guess.

Yeah axially sorry, luckily you knew what I meant.

As you increase cutter diameter you can push harder but with only one cutter I would play it safe.

When drilling you can go slightly higher chipload.

You could use a proper drill to rough out the slot maybe use a 1.2mm drill.

Then use the mill to thin the web and cleanup the walls.

I would go the full depth on the walls.

All my experience comes in an industrial environment over 20 years.

Phil

Sent from my HTC Desire using Tapatalk

Jonathan
15-01-2011, 09:12 PM
As you increase cutter diameter you can push harder but with only one cutter I would play it safe.

When drilling you can go slightly higher chipload.

You could use a proper drill to rough out the slot maybe use a 1.2mm drill.

Then use the mill to thin the web and cleanup the walls.


Higher chipload when drilling sounds logical due to being stronger axially, also I think the cutting edges on a drill are acute less acute angle so stronger ...
Anyway, I like the idea of 1.2mm drill since I've got plenty of carbide drills that size and one HSS. Due to the point angle on a drill I could actually squeeze in 1.8mm drill.

Time to add a drilling cycle I guess, more calculations...

Thanks for the advice.

Robin Hewitt
15-01-2011, 09:48 PM
If you are cutting teeth, have you considered a small slitting saw in a wide arbor?

They may bend but they don't break (unless you have a Z whoopsy) :naughty:

Jonathan
15-01-2011, 09:56 PM
If you are cutting teeth, have you considered a small slitting saw in a wide arbor?

They may bend but they don't break (unless you have a Z whoopsy) :naughty:

Yes I have considered that - it would be a lot faster. I've got a 1mm slitting saw that would do the trick.

The reason I've not done it is I've not got a tailstock for my rotary table and the pulley would have to stick out a fair distance for the slitting saw to clear the rotary table chuck. Maybe I'm being overly careful...

One nice thing is I can use almost the same gcode with slitting saw, just need to swap Y and Z axis.

blackburn mark
16-01-2011, 10:42 AM
All my experience comes in an industrial environment over 20 years.

dont let that intimidate you jonathan, in this country it could easy mean spending 15 years with a cup o tea in one hand and a fag in the other and wondering which hand to scratch your arse with :rofl:

looks like you missed a tooth on that pully?
parts for my 4th should turn up any day now :)

M250cnc
16-01-2011, 10:51 AM
dont let that intimidate you jonathan, in this country it could easy mean spending 15 years with a cup o tea in one hand and a fag in the other and wondering which hand to scratch your arse

Probably true in your case Mark

Phil



Sent from my HTC Desire using Tapatalk

blackburn mark
16-01-2011, 10:56 AM
indeed... i speak from experience :)

Robin Hewitt
16-01-2011, 12:02 PM
Since the advent of CNC there is a lot more fag smoking, tea drinking and arse scratching time available and you probably aren't encumbered by leather gloves set in a permanent clench. You can even smoke real fags instead of rollies because you aren't depending on it going out when you suddenly get busy with monotonous regularity.

We aren't newbies, we all know the problems with aluminium are it's bad habit of clagging the cutting edge and extruding when you want it to cut.

When faced with a tiny tool we also start to get nagging doubts about being able to transfer enough power to the tip. Watts = radians/second * Nm and the more Watts the more it is going to bend and once it starts to bend significantly, the more the chance of overloading it with a dig in.

I haven't found sub 3mm tooling in high helix with a rebate on the flutes and the carbide tinies tend to be coated with other than aluminium nitride so that helps not a lot.

Add to that the impossibility of getting anywhere near the correct cutting speed. If you could do 50k rpm the enormous feed rates required to maintain a cut above collet/tool eccentricity means you know that ain't going to work.

Even so, I wouldn't step drill it. Presumably you've turned a blank for the pulley and removed any surface hardening from the extrusion, if it isn't cast, and there is no oxide layer to wear an inconvenient slot in the flutes. Personally I'd go for around 2000 rpm, feed it at 1 -> 1.5 mm/s on a 3 flute, start with .25mm DOC, increasing if it seems good to go.

Standing over it with a blow gun, a pot of Rocol RTD and a brush could be an exceptionally good idea even if this temporarily suspends tea, fags and scratching :smile:

blackburn mark
16-01-2011, 12:46 PM
leather gloves set in a permanent clench

hahahahahaha!!!! i remember them
they where cold and uggly first thing on a winters a morning and you had to curl your fingers to get them in but it was allways heart breaking when you had to trade them in for a new pair :)
everyone seems to be using latex now, not the same (i must be getting old)

Jonathan
16-01-2011, 12:57 PM
Probably true in your case Mark


:rofl:



I haven't found sub 3mm tooling in high helix with a rebate on the flutes and the carbide tinies tend to be coated with other than aluminium nitride so that helps not a lot.

That sentence took me a bit of time to decipher!


Even so, I wouldn't step drill it. Presumably you've turned a blank for the pulley and removed any surface hardening from the extrusion, if it isn't cast, and there is no oxide layer to wear an inconvenient slot in the flutes. Personally I'd go for around 2000 rpm, feed it at 1 -> 1.5 mm/s on a 3 flute, start with .25mm DOC, increasing if it seems good to go.

Yes I'm using aluminum bar, not cast. I wasn't aware of surface hardening being an issue with aluminum (iron yes), however now you mention it it makes sense. One anodises aluminum to make the surface harder (or prettier), so it follows logically that the natural layer of aluminum oxide will wear the tool.

42T pulley with 0.25mm DOC and 1.5mm/s will take 170 mins. Maybe a little less if I get rid of some rapids in Gcode, but not much.
Chip thinning may enable me to run the cutter a bit faster for the same chipload a significant amount of the time. I can quite easily add that to my program.

I'm warming to the make a tailstock (anyone got a spare!) and just use slitting saw idea. I can stop the 63mm slitting saw bending by machining some 50mm steel disks and sandwiching it between those on the arbor.


Standing over it with a blow gun, a pot of Rocol RTD and a brush could be an exceptionally good idea even if this temporarily suspends tea, fags and scratching :smile:

Who says I can't drink tea whilst doing that!

Robin Hewitt
16-01-2011, 03:12 PM
That sentence took me a bit of time to decipher!


At risk of sounding patronising, I suppose it would be sociable on an open forum to explain that there is a difference when it comes to aluminium :naughty:

I've just taken a picture, two 3mm cutters designed for aluminium, one ordinary, 1mm, 3 flute carbide slot drill :smile: