Hello Guest it is January 29, 2020, 11:50:14 AM

Author Topic: I Keep Breaking Engraving Bits....  (Read 9706 times)

0 Members and 1 Guest are viewing this topic.

I Keep Breaking Engraving Bits....
« on: May 08, 2011, 04:44:30 AM »
I've been running my Taig CNC and every time I try and engrave, I end up breaking bits. I'm setting my code to do .001" per pass and 3IPM. I'm trying to engrave a piece of hardened steel (Uzi bolt) and it started engraving fine, but then the bits chip. I usually get about 20% of the way through before they break. What is the best way to fix this? Slower passes? Faster spindle speed? Cut less per pass? Any help would be GREATLY appreciated.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: I Keep Breaking Engraving Bits....
« Reply #1 on: May 08, 2011, 05:04:31 AM »
What dia/style  cutter, is cutter carbide or HSS is it coated or not?

I use the wee programme called Machinists mate which works well for me to give ball park figures for feeds and speeds.
Hood
Re: I Keep Breaking Engraving Bits....
« Reply #2 on: May 08, 2011, 05:08:17 AM »
# Geometry - 2-fute, 4-flute, "V" point
# Tip diameter nominal ±0.0002"
# Operating RPM - CNC certified operation 20k RPM to 100k RPM
# Ring Set - 0.800 in. ± 0.002 in. (optional)
# Material - solid submicrograin carbide
# Anticipated Life - 6,000 linear inches (fiberglass, CNC milling)
# Max. depth of cut - EFL varies by tip angle
# Runout (TIR) - 0.0002 in. max
# Shank dia. - 0.1250 in. (3.18 mm) +0.00, -0.0002 in.
# Tip angle - nominal ± 0.5°
# Length - indicated ±0.010 in. (30° 1.50 in. ±0.010 in.)

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: I Keep Breaking Engraving Bits....
« Reply #3 on: May 08, 2011, 05:18:28 AM »
Vee bits are sort of hard for me to get a real handle on feed and speed but your numbers look roughly what I would start at I think but that is dependant on your spindle speed. 10,000 rpm would seem to me to be a good starting point with maybe a slightly slower fpm, 2 to 2.5IPM.
A  great deal depends on the rigidity of your setup, especially with carbide as it is a hard material  but very brittle and easily chipped.
I am however not a trained machinist so take all I have said with a pinch of salt.
Hood

Offline Graham Waterworth

*
  • *
  •  1,934 1,934
  • Yorkshire Dales, England
    • View Profile
Re: I Keep Breaking Engraving Bits....
« Reply #4 on: May 08, 2011, 05:43:33 AM »
In hard materials you need to be above 20,000 rpm and the feed should be no more than 1/4 the tip dia per rev and depth of cut 1/3 tip dia.

I have had good results based on this but the machines are also very rigid so only a guide.

Graham
Without engineers the world stops

Offline RICH

*
  • *
  •  7,403 7,403
    • View Profile
Re: I Keep Breaking Engraving Bits....
« Reply #5 on: May 08, 2011, 09:47:06 AM »
If the tip is just .0002" ? then that will break by looking at it. I have tried down to about 2 thou and the point even breaks in Al.
Hardened recievers and parts usualy have the temper removed, are engraved, and then rehardened  or they are are done before hardening.
The tempering should be done by a pro with appropriate equipment. You should have a very slow feed rate to try and avoid chipping or breaking the tip since you want to have the cutter "cut" into the material  before it will move in some direction. Not much "impact" is required to break the tip.
As a test you may want to try a very slow feed into the material ......then inspect the tip to see if it has been chipped....if chipped then the cutting edge is gone and tool life will be short. You inpsect the tip with a microscope.
You really need an accurate machine ....there is a big difference between .001" plunge and say .0015" like wise for even smaller depths.
You may want to contact the manufacturer of the cutter and see what they recomend for the application. They will probably ask you
what the hardness is of the part.
FWIW,
RICH
Re: I Keep Breaking Engraving Bits....
« Reply #6 on: May 08, 2011, 10:58:54 AM »
Have you checkey the run out of your spindle.

0.0005 run out is enough to break the tip.

Did you tried acid etching, work great on hardened material.


Jeff

Offline Jeff_Birt

*
  •  1,107 1,107
    • View Profile
    • Soigeneris
Re: I Keep Breaking Engraving Bits....
« Reply #7 on: May 08, 2011, 11:31:32 AM »
I've used these same carbide 'V' bits in everything from Al to Stainless, but hardened steel may present its own challenges. Just a point of clarification, these bits have a 0.005" tip web +- 0.0002", not a 0.0002" dia tip. A 'V' bit has the advantage of giving you a small cutting area combined with the greater strength provides by the 'V' cross section.

On 303 stainless I was running the spindle at 7,000-8,000 RPM and feeding about 3ipm (plunge speed about 0.5 IPM as I recall) with a 0.001" DOC. With a harder material you may need to lower the depth of cut even more and speed even more. Also it is vital that you use a cutting fluid during the entire process.

I have a few 45 degree 'V' bits with 0.008" tip webs on hand. They are a bit stronger at the tip and might do a better job but I have not tried them on hardened steel. I'll send you one if you want to try it.

Happy machining , Jeff Birt
 
Re: I Keep Breaking Engraving Bits....
« Reply #8 on: May 08, 2011, 04:35:34 PM »
Well, I think I figured out a bit of my problem. When setting up what I want engraved in CamBam and transferring the G-Code, It seems that the measurements are getting magnified. I wouldn't think it would be so difficult. All I am trying to engrave is:

Stoner Arms LLC
Keizer, OR

And it needs to be .003" deep and the letters need to be 3/16" tall. Oh well.....back to the drawing board.

Offline Jeff_Birt

*
  •  1,107 1,107
    • View Profile
    • Soigeneris
Re: I Keep Breaking Engraving Bits....
« Reply #9 on: May 08, 2011, 06:26:56 PM »
Can you attach your CamBam file? I'll have a look at it for you.
Happy machining , Jeff Birt