Using tiny cutters (0.062" dia)

B

borne2fly

Hot Rolled

Joined

Feb 7, 2008

Location

California

• Feb 19, 2011

• #1

I'm wondering how much material I can remove in a pass with something this small? The workpiece is aluminum. Using a HSS tool currently set up to run at 22,000rpm and 100ipm. I'm ready to take off 0.005" per pass with the side, or 0.005" with the face using a 50% stepover. These little cutters look awfully delicate and I have no experience with them except the few I broke as a kid fiddling with Dremels.

 

D

Dimitri

Titanium

Joined

Jan 11, 2006

Location

Southern Ontario

• Feb 19, 2011

• #2

When using Frank Mari's tiny 3/64th endmills on copper, .0003 feed per tooth, at 4,000RPM (Max for the college's TM-1), and plenty of compressed air and cutting oil. Seemed to work. Anything much faster then that and all you heard was a ping and the endmill cutting air.

Dimitri

 

kapps

Cast Iron

Joined

Sep 17, 2007

Location

Orlando, FL

• Feb 19, 2011

• #3

Agreed. I was limited to 3500 rpm and I ended up running around 1.5-2 ipm in aluminum if I remember correctly. Blast it with air to get the chips out and spray with WD40 every once in a while.

 

B

borne2fly

Hot Rolled

Joined

Feb 7, 2008

Location

California

• Feb 19, 2011

• #4

So even at 20000rpm it looks like I need to keep it down to around 12 ipm. That sounds a lot more realistic than the 100 ipm I was looking at before. Thanks for the replies ........ you guys just saved me some bucks in broken cutters!

 

A

Armenius

Cast Iron

Joined

Jan 2, 2008

Location

S-W Ontario

• Feb 20, 2011

• #5

What kind of endmill are you running? Single lip or multiple lip?

The reason I ask is that cutter run-out becomes exceedingly important with small endmills.

As was pointed out above the CPT (chip per tooth) is on the order of .0003".

Imagine a 3 tooth endmill being fed at .001" per revolution. If this endmill has a run-out of .001" the feed per revolution will no longer be evenly distributed among the cutter's edges.

In the extreme one cutting edge does all the cutting and the cutter is now overloaded and breaks.

Moral of the story: Check the runout of small cutters and correct it if it is a significant fraction of the chip-per-tooth for that cutter.

Arminius

 

B

borne2fly

Hot Rolled

Joined

Feb 7, 2008

Location

California

• Feb 20, 2011

• #6

It's a 2-flute Niagra cutter, 0.062dia, 1/8 shank. I hadn't thought about the runout creating a problem, I'll definitely check it out. The smallest one I'm running is 0.031" dia, and at the moment I'm limited to 20,000rpm.
Some guys attach air driven pencil grinders to the quill to get over 50,000rpm, something I've considered. I've heard these little air tools can have runout problems, but I don't know if they were talking about the tool, or the cutter, or the combo.

 

S

Screwmachine

Titanium

Joined

Mar 8, 2001

Location

Switzerland

• Feb 20, 2011

• #7

Keep in mind that chipload is the most important thing: if you can get up to 50K you still need to be sure that you are in the ballpark of .0003" per tooth. Otherwise you'll be rubbing rather than cutting and tool life will only be slightly longer than if you overloaded it and broke it.

 

B

BobWarfield

Hot Rolled

Joined

Mar 4, 2006

Location

Northern California

• Feb 20, 2011

• #8

For 20K rpm, run about 19 IPM for 0.00047 ipt. That's if you have a really good spindle. The more runout, the less chipload you can run. Think of the runout as a % of chipload as it has that effect on the cutter.

Cheers,

BW
CNC Cookbook: Blog

 

A

adama

Diamond

Joined

Dec 28, 2004

Location

uk

• Feb 20, 2011

• #9

Don't run 50% step over, less or more but 50% is really nasty to cutters irrespective of size.

 

B

borne2fly

Hot Rolled

Joined

Feb 7, 2008

Location

California

• Feb 22, 2011

• #10

I can run it at 40% stepover, is that still too much?

Bob .... how did you calculate that 19ipm number? I still don't understand much of that stuff. I plan on plunging down .005 and then horizontally. Does chip load take into account the length of cut?

I can see I will need to check my spindle runout as a first step. In this case that means the runout of the Dumore die grinder .... it's strapped in parallel with the mill quill.

 

A

adama

Diamond

Joined

Dec 28, 2004

Location

uk

• Feb 23, 2011

• #11

Go look in the cnc section and do some searching on step over. There's a lot of info there and it does make a real difference to cutter life. Sandvick have some good you tube videos too on cutter entry and step over. Equally look into chip thinning.

There all basic ideas than can be applied to anything from a mill drill right up to a 5 axis machining centre. Equaly the concepts work on cutters of any size, just scale feeds - speeds accordingly.

 

macona

Diamond

Joined

Jun 20, 2006

Location

Beaverton, OR

• Feb 23, 2011

• #12

NSK makes a nice little air powered spindle, but I think they are around $3k. But they need a big compressor to keep up.

Fischer Precise makes some nice electric spindles that will go way up there. I have one and it works nice. ABEC 9 bearings in it.

 

B

borne2fly

Hot Rolled

Joined

Feb 7, 2008

Location

California

• Feb 24, 2011

• #13

Those air spindles are nice, but way out of my price range for now. I'm going to have to make do with what I have.

 

P

Piecemaker

Plastic

Joined

Apr 24, 2010

Location

Alabaster, Alabama

• Mar 30, 2011

• #14

the tinies

I know that im late on this one but I do alot of pocket type engraving in aluminum and with a coated carbide 1/32 4 flute I can run 66% stepover at .025 deep at 1 ipm. at 1.2 they're history. they also seem to last forever as long as they have slow running coolant bath. I run a 1/16 4 flute at 2 ipm at .05 deep. they will cut at 2.5 or even 3 ipm but it has bit me in the ass a few times. I am open for suggestions if anyone has any. I got a 100 piece job in the works at 100$ a pop. This time, time really is money!

 

P

Piecemaker

Plastic

Joined

Apr 24, 2010

Location

Alabaster, Alabama

• Mar 30, 2011

• #15

I know I need a high speed spindle. the dough from this job will buy one.

 

W

willbird

Banned

Joined

Jul 19, 2005

Location

North(very) West(very) Ohio...near exit 13 on OH t

• Mar 30, 2011

• #16

Armenius said:

What kind of endmill are you running? Single lip or multiple lip?

The reason I ask is that cutter run-out becomes exceedingly important with small endmills.

As was pointed out above the CPT (chip per tooth) is on the order of .0003".

Imagine a 3 tooth endmill being fed at .001" per revolution. If this endmill has a run-out of .001" the feed per revolution will no longer be evenly distributed among the cutter's edges.

In the extreme one cutting edge does all the cutting and the cutter is now overloaded and breaks.

Moral of the story: Check the runout of small cutters and correct it if it is a significant fraction of the chip-per-tooth for that cutter.

Arminius

Click to expand...

Sometimes you cannot do much about runout, but one thing you CAN do is grind another setscrew flat and index the cutter 180 degrees and get more life out of it. In some shops tool holder selection is often limited, and there is not much you can do about it.