Author Topic: CNC engraving text  (Read 1406 times)

Offline gldavison

  • Full Member
  • ****
  • Posts: 219
  • Tarkio, Mo.
CNC engraving text
« on: October 25, 2022, 01:56:42 AM »
What feed rate would you CNC 'ers use on these 20 degree v bits?  My first attempt finial 0.050" plunge rate 10"per minute. The point broke as soon as it touched the aluminum. Feed rate was set at 30pm. Second attempt finial 0.050" plunge rate 5"pm, feed 15"pm, point didn't last one letter. DOC was 0.015". My spindle max's out just short of 10,000rpm.  Before I break any more bits, i thought I would ask for some advice.


https://www.amazon.com/SainSmart-Genmitsu-Engraving-Degree-Conical/dp/B07P71RDPL?pd_rd_w=tFEkK&content-id=amzn1.sym.bcca84ef-5f4d-4682-852e-b0b38f16e8ba&pf_rd_p=bcca84ef-5f4d-4682-852e-b0b38f16e8ba&pf_rd_r=XA6R66HXV1MYSYZN7VCK&pd_rd_wg=QGCmE&pd_rd_r=f746d788-a35a-41d8-847b-e21537462a6d&pd_rd_i=B07P71RDPL&psc=1&ref_=pd_bap_d_csi_pb_allspark_BIA_1_i

Gary
Gary
Windows 10 & 11, Alibre Design Pro V27, IntelliCADPro6, CamBam, Mach4, 3D Printers, Cetus, Anet ET5 X
15" South Bend, 10" Logan lathe, Grizzly square column mill, CNC router & Hot wire cutter. Lagun FTV-1 knee mill, Sherline mill & lathe

Offline steamer

  • Global Moderator
  • Full Member
  • *****
  • Posts: 12697
  • Central Massachusetts, USA
Re: CNC engraving text
« Reply #1 on: October 25, 2022, 02:52:00 AM »
For the engraving on the vise project, I was running at 10,000 rpm,  .03" DOC, and 3 in/min in brass with a 60 degree engraving tool.  ( carbide)

No issues
"Mister M'Andrew, don't you think steam spoils romance at sea?"
Damned ijjit!

Offline john mills

  • Full Member
  • ****
  • Posts: 417
Re: CNC engraving text
« Reply #2 on: October 25, 2022, 03:55:38 AM »
what is the tool you have ?are you using coolant?
I did lots of engraving mainly in tool steel  MST for embossing dies years ago Iground D bits as best I could with the tools i could use.
the first machine had spay mist coolant latter machines ordinary coolant supply .the tools were just hss spindle speed only just over 3,000rpm  don't remember the feed possibly 40 mm /min.latter i run a machine with a 10000 rpm and good flow of coolant i think 200mm/min feed the boss did want nothing to do with D bits and would only supply ball nose carbide that was for aluminium.
i found the important part was to get a tool that run as true as possible D bits don't have much clearance and a little bit out the tool would fail.some would last a long time and some did not so it was good to get good at grinding them .The ball nose end mills lasted alright but
it was for aluminium with a good flow of coolant better than most machines have .its surprising how high the feed could be.The right g codes
to cancel the acceleration and slowing between lines in the program.
John   

Offline Hugh Currin

  • Full Member
  • ****
  • Posts: 720
  • Box Elder, SD, USA
    • www.currin.us
Re: CNC engraving text
« Reply #3 on: October 25, 2022, 04:47:52 AM »
Gary:

I haven't done much engraving but here's my two cents worth. I see that tool has a 20deg included angle with a flat tip of .004". Carbide single flute cutter, single cutting edge. At 0.015" depth of cut I find the tool diameter at the surface to have a diameter of about 0.0093", darn small. Let's assume, if we're cutting mild steel, the cutting speed should be something like 500 SFPM (Google) or 6000 in/min. Thus we should have the god awful high speed of 1,304,000 rpm. The cut per tooth, again from Google, is maybe 0.0006" for an 1/8" endmill. Looks like we should use less for a smaller tool so here let's use 0.0004". So 0.0004" per revolution, single flute, gives a feed rate of 520 in/min. I think this will scale so at 10,000rpm we should use 10000/1304000 = .0077 of 520ipm, or 4ipm.

I'd start at full speed, 10,000 rpm, and maybe 2 or 3 ipm. Seems reasonable for a tiny tool. (I think your speed is way too slow if, as you say, it's 30 rpm.

Hopefully someone else will give you better insight. Thanks.

What feed rate would you CNC 'ers use on these 20 degree v bits? ..... Feed rate was set at 30pm. Second attempt finial 0.050" plunge rate 5"pm, feed 15"pm, point didn't last one letter. DOC was 0.015". My spindle max's out just short of 10,000rpm.

Gary
Hugh

Online Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: CNC engraving text
« Reply #4 on: October 25, 2022, 07:12:39 AM »
Again. I've not done much engraving with this type of tool but what I have done was in brass, at my max spindle speed of 5000rpm and a feed rate of 50mm/min and depth of 0.1mm so thats approx 2" feed and 4thou DOC at your 10,000rpm feed could be double.

Stopping material sticking to the bit with aluminium will be something to watch, mist of flood by hand

Offline maury

  • Full Member
  • ****
  • Posts: 515
    • Lone Star Engine Works
Re: CNC engraving text
« Reply #5 on: October 25, 2022, 02:02:24 PM »
I was CNC engraving nameplates for the Forest kits I once produced. I used a V bit that was fixed in the tool holder- not spring loaded. I found I had to make a pocket or facing cut first to get the surface flat with the XY plane. Don't remember the speed, but the depth was about .010". never broke a tool, If you cut .001 per turn of the tool you should be ok on speed.
maury
Lone Star Engine Works retired.
"The trouble with socialism is that you eventually run out of other people's money."... Margaret Thatcher

Offline kvom

  • Full Member
  • *****
  • Posts: 2649
Re: CNC engraving text
« Reply #6 on: October 25, 2022, 03:19:55 PM »
G-Wizard gives 5 ipm, 2 ipm plunge.  That's maximum.  Fine Finish drops feed to 4.4 ipm.  Coat surface with WD40 to prevent sticking.

Offline dieselpilot

  • Full Member
  • ****
  • Posts: 341
Re: CNC engraving text
« Reply #7 on: October 26, 2022, 12:16:31 AM »
If engraving .050" deep to achieve line width, I suggest a tool with a larger angle. I use a 90°, .005" tool to engrave 3/32" tall text.

Offline gldavison

  • Full Member
  • ****
  • Posts: 219
  • Tarkio, Mo.
Re: CNC engraving text
« Reply #8 on: October 28, 2022, 12:55:28 AM »
Thanks for all the replies. Got-R-done.



As yo can see ,I made a center height gauge for my Sherline lathe. Wanted to make sure that piece did not get returned back to the scrap bin.

Plunge rate 1 ipm, feed 2.5 ipm doc 0.003. Filled with red Dykem.

Gary
Gary
Windows 10 & 11, Alibre Design Pro V27, IntelliCADPro6, CamBam, Mach4, 3D Printers, Cetus, Anet ET5 X
15" South Bend, 10" Logan lathe, Grizzly square column mill, CNC router & Hot wire cutter. Lagun FTV-1 knee mill, Sherline mill & lathe

Offline Admiral_dk

  • Full Member
  • *****
  • Posts: 3752
  • Søften - Denmark
Re: CNC engraving text
« Reply #9 on: October 28, 2022, 10:36:17 AM »
Great idea and execution - ie. I can read it  ;D   :old:   :ThumbsUp:

Per

 

SimplePortal 2.3.5 © 2008-2012, SimplePortal