CNC Helix?

[Steve355Participant @steve355]

I broke an endmill on Friday. I was trying to helix a M2 clearance hole in 1mm brass (cz108), which is basically a 2.1 mm hole using a 2mm endmill. So it is very tight, and using my usual feed rate (12 IPM I think) translates to more of an excited wobble than a nice helix. I wasn’t tremendously surprised when the tool broke.

Any tips on CNCing such a hole in a serene fashion  without breaking end mills?

 

cheers

[mike TParticipant @miket56243]

Try a feed rate of 1 inch per minute.

[John HaineParticipant @johnhaine32865]

12 ipm is 300mm/minute!!!  I’m not surprised it broke!  Yesterday I spiral drilled 6 5mm holes with a 3mm endmill at .3mm pitch and 100mm/min feedrate.  No drama, nothing broke.  I’ve had 1mm endmills break trying to spiral when I forgot to change the feedrate from its default 800mm/min.

 

[JasonBModerator @jasonb]

You don’t say what your cutting speed was or how many flutes as that will affect the chip load, 300mm/min could be fine if you are at 10,000rpm or more.

When doing a helix you need to take into account that the feed rate is based on the centre of the tool. So in a cas elike this where the tool diameter is clos eto the hole diameter the feed rate at the cutting edge is considerably more

1.1mm circlular path ha sa length of 3.45mm.

Your hole edge at 2.1mm dia has a circumference of 6.60mm.

So the edge of your tool is traveling at almost double the feed rate of the middle. eg 600mm/min..

You don’t say what the depth is but you also need to allow time for swarf to get out when the tool is taking up most of the room

 

[Julie AnnParticipant @julieann]

For all intents and purposes the cutter is not following a helix but is plunging straight down. So the centre of the cutter is working at zero cutting speed. Professional guidance is that for helical ramping the cutter diameter should be a maximum of half the hole diameter. So use a 1mm diameter cutter.

Feedrate is dependent on spindle speed; I will run a 1mm diameter cutter at 300mm/min, but at a spindle speed of 24000rpm.

Julie

[Steve355Participant @steve355]

That’s interesting, yes in effect it is plunging straight down, but unlike a drill, it is drawing a circle as it does. I could try drilling instead of a helix but I’ve had poor results (broken end mills) with that in the past.

Ive been running it at 12000 rpm.

It’s 0.9mm thickness brass. Most of the swarf seems to be evacuated, most of the time.

So, looks like I am ordering some 1mm cutters and running it at 24000. Thanks Julie I will give that a try.

Steve

[JasonBModerator @jasonb]

If it is just a clearance hole is there any reason why you can’t just put a 2.1mm drill bit in the machine and drill the hole?

I had assumed you were boring it to save changing cutters with the 2mm being used for other machining ops but if you are changing to a 1mm cutter may as well change to a 2.1mm drill and have a tool that is less fragile and will do the job quicker than a 1mm milling cutter that will still need a relatively slow feed.

Mine will do 2.1 drilled holes without problems at 5000rpm in all materials a size I use for tapping M2.5

If you don’t have a 2.1mm drill or want a milled finish then just run a 2mm drilled hole first and finish with the 2mm milling cutter to 2.1mm.

[Steve355Participant @steve355]

Actually, that originally was the case as I was using the 2mm endmill for profiling operations also. But I broke too many of them, so switched to 3mm for profiling. Whether I’d have broken so many now I have my special blower, is a question.

But I can’t avoid needing 2.1mm holes for clearance, so I’ve been switching the endmill just for that.

But yes I could try a drilling operation instead, as you say, using a drill bit rather than an end mill.

Whichever way I do it I have 4 tool changes to make the part, which is a total pain. I’ve been messing around with this for weeks now 😒

[JasonBModerator @jasonb]

I make a lot of models with metric fixings and all my “clearance” holes are drilled nominal size so for M2 I just drill 2mm. Never had a problem putting engines together even with multiple long studs with just the ends threaded.

If I am drilling holes to hold a job in place for further machining I measure the screws and drill to suit. 2.9mm works fine for M3 cap heads.

[Steve355Participant @steve355]

In practice most of the drill bits I own seem to be very slightly oversized, I guess because of you bought a 2mm drill bit and couldn’t get a 2mm screw through the hole it makes you’d be annoyed.

The problem I’ve had with using drill bits on a milling machine is them drifting off target. I ended up measuring blueing and punching manually to stop the drill wandering.

[JasonBModerator @jasonb]

I’m the opposite and hardly ever mark out these days. I tend to use an edge finder and DRO to position things on the mills and the drill press never really gets used to drill holes. If I do mark out it is usually just to work out the best placement in a casting which can be a case of placed to suit rather than place to measurement, even then I won’t punch but just eye up the drill over the mark or use a wobbler where it matters a bit more.

I would say 95% of the time I don’t even spot drill, I just go straight at it with a stub drill usually held in a collet unless I need a deeper hole in which case I spot and then use a standard jobber length drill. That applies to the manual mills as well as the CNC.

My drill bits of choice are Dormer A022 for the stubs and A002 for jobber length, these are “split point” and really don’t need spotting first.

I don’t seem to get problems with wandering, items drilled with a PCD Hole pattern tend to fit in any position and can be flipped over and still fit and that is with my smaller clearance hole. That is in a mix of steel, cast iron, brass, bronze & aluminium.

[Author]

Posts