Engraving.....TM Series

[behindpropeller]

I have never done any Engraving.

Can anybody give some advice?

Feeds/speeds?

Thanks

Tim

[Donkey Hotey]

I generally spin it to death (max RPM). 10 IPM. Engraving depth between 0.006 and 0.008 for small stuff (letters under 0.5" tall). Bigger than that and 0.010" deep makes it a bit more readable.

[Geof]

On 6061 I feed at 30ipm to 40ipm using a 90 degree carbide spot drill as the tool. The machine tends to shake a bit at this feed but the engraving is very nice.

[Donkey Hotey]

So you're really just dragging the cutter through the aluminum, right? At the cutting point, there ain't much going on in the way of chip clearance.

I wonder how it would be just dragging a diamond cutter at any old RPM.

At the Haas demo day last week, they were running one demo with very fine engraving at about 30 IPM and it was gorgeous. I never did find out what kind of cutter they were using.

[Geof]

I think 'proper' engraving tools are a single cutting edge for better chip clearance but they have to be spun very fast. Tiny spot drills work quite well, for letters less than .2" a 1/8" spot is best but for larger lettering 1/4" is okay. I have tried using small ball nose cutters and they give a beautiful polished finish, probably because they rub so much, but they break very easily. A very nice effect for larger lettering is colored anodizing followed by engraving using a corner radius (bull) endmill just going deep enough to strip off the anodizing.

[helocat]

Tim - I just used the IPS engraving tool today for the first time. It's been just over 12 yrs since I did any engraving with a mill. But it came back to me. Like Geof said, I used a #4 center drill that had a .120 tip on it. I did use the auto speeds and feed calculator in the tool set up page for .120 "drill" with two flutes. I also remembered to run a shell mill for a nice clean up pass on the material to make sure the engraving is uniform. Like Geof talked about with the after machining of an anodized part, this is real key to have good square parts to reload so that there is no hight change. With such a light depth of cut a few .001 is real visible with after machining. (I recall years ago fighting inconsistencies on some promo parts we were after machining that had one side w/ mill scale)

So today I loaded the text, called up .25" letters and set my G54 Z offset 1" above my part and ran the program to see how long the text was. I then moved my G54 offset to better accommodate the text to where I wanted it, removed my 1" Z offset and let her fly. I did one pass with a .010" depth of cut, then ran it again at .020". Looks great! Now I want G51 even more for my company logo.

Mark


Here is the first part I made on the new mill and the engraving: (Custom transfer case center mount. Sides will be welded to it and bent tube for the rest of the supports.)



Uploaded with ImageShack.us

[CC12v]

I have a TM3P, 6000 rpm ,25 ipm feed and plunge on 6061.
1/16th ball.There are better tools but this gets the job done.

[HelicopterJohn]

Here are a few pictures of an engraving project I recently completed and another one I am working on.

I used a .125 2 flute ball end mill to cut the grooves in the STAR gameboard. The material was plexiglas.

I haven't cut the helicopter clock yet as I am trying to decide on the color of translucent plexiglas for the project. I hope to have it backlit in a shadow box.

Just a couple of fun projects that I produced utilizing my ONECNC CAD/CAM software.

John

[Vern Smith]

Nice John, your an artist as well as a machinist

Vern

[Matt@RFR]

I've been using a 1/32" 2 flute ball nose for my engraving. I like ball nose endmills because you don't have to go very deep to get nice wide, readable letters.

12k RPM, up to 80 IPM for rough stuff down to 40 IPM for finer things, usually .003" to .005" deep. Any deeper and I start backing the feed down, or for prototypes, atleast run a spring pass. This is all for 6061, but I've been using the same tool for all my engraving for the past year or so...not the same type of tool, the same tool.

The only downside to using ball nose endmills for engraving is that they are very, very touchy to having a very flat surface to engrave on, otherwise the width of your letters can have big discrepancies.

One thing that will help your engraving cycle times immensely is to use a clearance retract of whatever you're used to (say .25"), but put your retract plane to .010" and your feed plane to .005". If I do my normal .25" / .1" planes, not only is it slower, but the machine really bangs around a lot everytime the Z rapids up then down.

[HelicopterJohn]

Hi Matt,

Thanks for the tip on the Planes. Just one of those things being a novice that I tend to forget.

John

[helocat]

Originally Posted by HelicopterJohn Here are a few pictures of an engraving project I recently completed and another one I am working on. I used a .125 2 flute ball end mill to cut the grooves in the STAR gameboard. The material was plexiglas. I haven't cut the helicopter clock yet as I am trying to decide on the color of translucent plexiglas for the project. I hope to have it backlit in a shadow box. Just a couple of fun projects that I produced utilizing my ONECNC CAD/CAM software. John

I dig the clock! BK117? A bit of an EC135 front end...... nice.