O/T Engraving

[Joels]

I need to engrave 6061 Aluminum on a Fadal VMC. Can anybody recommend a cutter i can use? I was thinking of a ball endmill.

[jctjct]

we use carbide centerdrills for shallow letters.

[Joels]

i though about center drills but i was worried about the side load and breaking the tool. thank you for your input. i will be engraving shallow letters so i will give it a try.

[DavidB]

Get an old cutter and make a d-bit.

Cheap

 

[Phil Orenstein]

For centerline or fine engraving I use sharp V Cutters with a 30 deg included angle ground on a Dekel with a .002 - .005 tip. Crank up the Fadal to 10,000 RPM if it will go that high and feed at 10 IPM or slower. Very small DOC like .001 or .002. Let her run all nite!

 

HTH

Phil

[crazy^millman]

+ on Phil but I prefer a 60 degree included angle for my engraving. I have also used ball endmills and if on a curved surface like the results of a ball over anything.

 

HTH

[Midwest]

For engraving I take an 1/8 dia carbide round or old em shank and grind a 3 sided pyramid cutter. I set the cutter grinder to 15 deg or 20 deg. most of the time and grind to a sharp piont. Step down of .002, step over of .004 for roughing and .001 - .002 for finishing. Feed of 10 ipm and a rpm 10,000. Cuts well in soft or hardened steel.

[Guest]

+1 on Midwest. I have used that type of cutter on many types of materials.

[DavidB]

I have had better results gringing the carbide to its centre line and at a 30° Inc angle than the pyramid type.

 

You can even purchase them double endded if you have no time.

 

[Joels]

Thank you all for your imput. We are not able to correctly grind tools in our shop. I will have to purchase these tools. Can you give me a idea of what to buy? this will be used to engrave letters on a flat piece of aluminum maybe .003 deep or less. this is for my boss so i has to be perfect. i am using a Fadal VMC 4020 pallet changer. 10000 RPM max

[DavidB]

I would contact your local tool supplier or look on the net.Im in Australia so I dont think my supplier info would help you.

 

I get double endded single lip cutters.

They are ground to the centre line. Once it gets dull just turn around and use the other end.

Be carfull handling them they are sharp

 

HTH

[Lars Christensen]

Watermaker,

I think most tool supliers cary them, try Ultra tool, Harvey or MSC etc.

 

Lars

[Smit]

We use the SGS CM000750, .03R X 7 DEG taper mill. .005 or .01 depth of cut, 38 IPM @ 6112 RPM. Works great for marking parts, and readily available from our vendor.

[Fig sign]

Midwest !

 

~~~~~~~~~~~~~~~~~

3 sided pyramid cutter. I set the cutter grinder to 15 deg or 20 deg. most of the time and grind to a sharp piont.

~~~~~~~~~~~~~~~~~~

I never grind to the sharp point ,No ,I grind to it ,but after that I take a little back angle

like 3-6 degrees to form little cutting dia at the bottom .

Tool life will be greater many times .( you can not mill with diameter Zero ).

Beeing lazy I do it by hand mostly (especially if I do it many times to get correct diameter )

HTH

ITHH

[Midwest]

Iskander teh Owl

 

Try it some time you might be surprized. The tip might chip with some carbides. I have one now that has cut a lot of engrving without chipping the tip. The tool has to run true to last.

 

[Chris Rizzo]

I prefer the MICRO 100 line of engraving tools. 60 degree included angle cutters seem to last longer than the 30 degree cutters...the tips are pretty fragile on those! On aluminum, full throttle on the spindle, .005-.01 DOC about 20-30 IPM. RSC-125-2 model It's the double ended model...

[cadcam]

Watermaker, you can get them from Marshall tool or Roy & Val can make you one up.

Both if for some resion you have not heard of them are in chatsworth.

 

I am not sure were in LA you are it is a big county.

[Philcott]

When using the double ended engravers be careful to not damage the tip on the non working end while putting it in the collet. Those tiny carbide tips will take NO abuse without chipping.

 

Phil

[Fig sign]

Midwest !

 

I doubt that I would check , most of my engarving nowadays are on copper ,steel,hardened steel and after even nitrocarbonizing(sometimes )

I have only 8000 rpm and did it in the past on 4000 rpm`s and in this materials chipping (as you call it ) is a must (IMHO).

And I do not have quantaties ,one-two parts max .

But I really will check at first possibility .

I am very sceptic ,I think your tip is broken a bit producing sorta chip aniway .

Have you seen it under microscope ?!?

It `s not a stubborness , only curiosity !

Regards

[Midwest]

Iskander teh Owl

 

After you run the tool you do get a very slight working edge. If the tool chips you can see it very easily. I started cutting with only 3000 rpm's a few years back, you just have to slow the feed rate down. We build molds so we also do low quantities.

[G Caputo]

No flaming or laughing here guys... One cheap option to get the rpm's up is to take a "c" or "d" series spade drill holder in your spindle. They got nice big grooves down the side for chip evacuation, which also doubles as a vee to hose clamp a die grinder in. Waalaa, 26000 or whatever those things spin, spindle. All we have here are big machines, so no high rpm spindles. 2600 on a 6" floor bar is the fastest. This works like a charm too, its'cheap, might be a little hillbillyish, but it gets the job done. I guess you could get a speed up head also..... but what fun would that be.

 

Greg

[JCLM]

I purchase engraving tools from a place called Harvey Tool. They work extremely well. They have a web site, www.harveytool.com

[mold100]

+1 on Harvey the tool I use is the 1/4 shank TiCN coated, its 18.30 in the book but 1/8 shank is only 9.80.

 

I actully prefer the 3 sided pyramid myself but dont like to %^&^$^ grind them up. So I just get'm from harvey