Broke a cutter, not sure why (G code in here)

This forum is dedicated to those Hobbyists Interested in CNC machining in their home shops. (Digital Read Outs are also topical, as is CAD/CAM as it relates to CNC)

Moderator: Harold_V

User avatar
ctwo
Posts: 2600
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Broke a cutter, not sure why (G code in here)

Post by ctwo » Sat Oct 01, 2016 7:55 pm

Basically, a 0.25" cutter is spiraling down 1500 RPM into steel at a slow rate, 7 ipm, creating a full width slot. I was using cutting oil and air to keep the chips clear and it was going well. Material is steel, a piece of 12" x 12" angle that was used as a large bracket for file cabinets. I cut out a smaller flat piece for this project, and it was clamped flat in the vise.

The first circle is ~1.5" diameter and starts at Z0 and progresses around to 0.070" depth. The cutter continues its decent around the second pass, now at constant depth of cut of 0.070" and continues round and round until the final pass, cutting all the way through at 0.390". Then there is another cut again at the surface with a 0.125" larger radius, two passes to achieve a depth of only 0.120".

Code: Select all

%
(cutter: 4 flute, 1/4")
(RPM: 1500)

G90
G00
Z1
X0 Y0
G00 X0.000 Y0.625 Z0.020
G1 F7
Z0
(CCW circle)
G03 X0.000 Y0.623 Z-0.070 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.140 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.210 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.280 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.350 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.380 I0.0 J-0.623
G01 X0.000 Y0.625
G03 X0.000 Y0.625 Z-0.390 I0.0 J-0.625
G00 Z0.010
G01 X0.000 Y0.750
G01 Z0.000
G03 X0.000 Y0.748 Z-0.070 I0.0 J-0.748
G03 X0.000 Y0.748 Z-0.120 I0.0 J-0.748
G01 X0.000 Y0.750
G03 X0.000 Y0.750 Z-0.120 I0.0 J-0.750
G00 Z1
X0 Y0
M30
%
OK, I'll tell you where it broke, but it would be nice if someone could tell me where I went wrong first. I have an idea, but do not want to influence your thoughts as I almost predicted the breaking point, but somehow felt confident it was OK. Doh!

Thanks!
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
GlennW
Posts: 6587
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Broke a cutter, not sure why (G code in here)

Post by GlennW » Sat Oct 01, 2016 9:00 pm

HSS, Cobalt, Carbide??

Was it a center cutting end mill?
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

Harold_V
Posts: 16804
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Broke a cutter, not sure why (G code in here)

Post by Harold_V » Sun Oct 02, 2016 1:17 am

I assume you created a plug, the center piece. if so, I expect the end mill broke when the plug fell free. It was likely dragged in to the cut (or directed there by the air blast) instead of falling out the bottom. Doesn't always happen, but it's certainly one of the hazards.

Harold
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
ctwo
Posts: 2600
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Broke a cutter, not sure why (G code in here)

Post by ctwo » Sun Oct 02, 2016 7:33 am

It was carbide and I think center cutting, although why would that matter? It broke right when executing the line of the second pass of the first circle, when it hit a depth of 0.070. The end just shattered.

I was first thinking that there would be irregular metal there, but concluded that should not be the case and carried on. I replaced the endmill, slowed the feed 50% and started again. After cleaning up the 3rd pass at 0.210, I started bumping up the feed to 80% and it was fine. I did slow the feed at the end of the last pass on this hole because I was also worried about the slug, but it managed to tilt and fall down without issue.

I use an Excel spreadsheet that lets me play with the numbers below and calculates some of the figures. I gave it a 20% margin before it will flag an out-of-bounds condition, and none were flagged. I was pushing it a bit, but still not sure why the cutter broke.

Cutter Diameter= 0.25
Flutes= 4
SFM= 98.25
RPM= 1500
Chip Load= 0.00117
IPR= 0.00467
IPM= 7


The ideal case it suggested was:
RPM= 1528
IPM= 6.11

Based on the values I enter below:
Cutter Diameter= 0.25
Flutes= 4
SFM= 100
Chip Load= 0.00100
Attachments
endmill-20161002_042305.jpg
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
Dave_C
Posts: 924
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: Broke a cutter, not sure why (G code in here)

Post by Dave_C » Sun Oct 02, 2016 1:49 pm

CTWO,

I think I see why the cutter broke on the second line.

There is nothing to stop the plunge from going in full speed! It made the first pass, then dropped without any ramp and end mills , small ones for sure, don't like to plunge cut at that feed rate.

Probably makes sense why it survived when you slowed the feed rate.

Maybe,

Dave C.
I learn something new every day! Problem is I forget two.

User avatar
GlennW
Posts: 6587
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Broke a cutter, not sure why (G code in here)

Post by GlennW » Sun Oct 02, 2016 2:35 pm

ctwo wrote:It was carbide and I think center cutting, although why would that matter?
It's not going to like plunging if it is not center cutting.

If it was carbide you were running it at HSS speed. Carbide likes about triple HSS speed.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

User avatar
ctwo
Posts: 2600
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Broke a cutter, not sure why (G code in here)

Post by ctwo » Mon Oct 03, 2016 3:17 am

Hi Folks,

The program does not plunge straight down. Each circle begins at the current Z and ends on that line's Z. In this image, the white line is the first pass, starting at the surface of the steel (at 1), ramping down CCW, and breaking at 2. The dotted red line is the return path after finishing the hole.

If using triple the SFM for carbide, then I get ~4500 RPM and 18 IPM.
Attachments
spiral.png
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
Pennsy fan
Posts: 715
Joined: Thu Jun 17, 2004 1:50 am
Location: North Hollywood,CA

Re: Broke a cutter, not sure why (G code in here)

Post by Pennsy fan » Mon Oct 03, 2016 10:25 am

After reading all of this I'm thinking my first take was the rpm was way to slow, plus not enough coolant. It's sounds like a chip recirculated and caused the damage. Also when ramping you want to use the biggest cutter you can, ramping Is a big load on smaller cutters.

User avatar
ctwo
Posts: 2600
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Broke a cutter, not sure why (G code in here)

Post by ctwo » Mon Oct 03, 2016 1:31 pm

No coolant, just hand held air and brushed cutting oil. (I need to get my mister installed.) You might have it there and the transition to the next line was just a fluke.

I didn't think carbide would get angry running too slow. Also, is a center cutting end mill required for ramping into a cut? I did not think it would be.
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
GlennW
Posts: 6587
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Broke a cutter, not sure why (G code in here)

Post by GlennW » Mon Oct 03, 2016 2:56 pm

I always use center cutting when ramping.

I also slow the feed rate a bit when ramping as you are loading the cutter differently than just side milling.

Chips don't always clear as well when ramping as they do when just side milling. Just like they don't clear as well when plunging without a pilot hole.

Edit to add the word "always"
Last edited by GlennW on Mon Oct 03, 2016 4:03 pm, edited 2 times in total.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

Harold_V
Posts: 16804
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Broke a cutter, not sure why (G code in here)

Post by Harold_V » Mon Oct 03, 2016 3:34 pm

ctwo wrote: is a center cutting end mill required for ramping into a cut? I did not think it would be.
It isn't required, but will usually offer better machining characteristics. I've ramped (manually, not with CNC) countless numbers of times with less than acceptable end geometry---with mixed results.

Harold
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
ctwo
Posts: 2600
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Broke a cutter, not sure why (G code in here)

Post by ctwo » Thu Dec 29, 2016 6:24 pm

I have not been doing enough practice, so I'm STILL breaking cutters. Seems like every time I use the machine...

Now I am cutting a 1/8" groove in an aluminum block. HSS 2-flute cutter, 3/16" shank and 3/4" long (cutting edge). Let's say all I want to do is drive from one end to the other.

3800 RPM
0.040 DOC
5 IPM
constant air and brush cutting oil (mix with kerosene)

Now, I'm expecting the EM to snap right off as soon as it touches aluminum, but it begins to plow through. It's going great until it comes out the other side and I hear the EM hitting something. The next pass I noticed the EM kind of flicked out of the groove, so it was flexing in the cut. I reduced to 4 IPM and less noise on exit, but EM still flexing and flicking out and it snapped exiting. 2 IPM same thing exiting and snap.

Now when I queue up youtube videos, I can see cutters like this jamming through aluminum at 400 IPM. Of course they are spinning 100k RPM, but what do I have to do to not go broke buying EMs? The feed already seems ridiculously slow.

p.s. the part is more complex than a simple groove, so that is why I am using an EM.
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

Post Reply