how to engrave

[cob]

can some tell me what is the kind and size of drills you use for engraving using mastercam

[an0n]

Usually engraving is done with engraving cutters and not drills as they do not cut very well and arent very rigid if you still want to try it you can try it with as short drill as possible. I think this should be interesting for you: http://www.antaresinc.net/FactCutterGeometry.html

[hummel]

you can also use an senterdrill. only 0.05mm down in piece. 4000-5000 rpm

[mberry]

Most of our Engraving is done on our Haas Mills using the Haas Macro Program that came with the Mill. We use a Centerless Ground Engraving Blank made by Garr Tool. This carbide blank is ground to a point by us and our depth of engraving is usually only .005 at most. Since our letters/numbers are not more than .125 in height this works well. I have used 118 deg drills for engraving larger characters and this has worked well also. The size of the drill can very greatly as long as it has a center cut tip.

[Paulo E.]

You can use a number of things to engrave. Generally there are tools for engraving alone, however if you want to save yourself some money, as some suggested, a #0 or #1 center drill, 1/16 ball end mill or even a spot drill depending on the size of the letters. It boils down to the size of the letters and the quality of it, if you want small letters and nice clean lines then you need a engraving tool, they generally have an acute angle and a small flat on the tip that allows for optimal material removal. Last but not least as engraving usualy ranges between .004 and .007 deep. staying with in those parameters and using high rpm usually yield the best results.

[Boots]

You can also engrave with a stylus in soft material like brass, gold, silver, etc. with zero RPM by just dragging. A lot of choices here.....

[BILLFUNK29]

A nice tool we use has a spring in it to allow the engraver depth to be controlled by pressure instead of Z depth. It gives a uniform depth on material that is out of flat up to .005".

[kuyohtay]

Someone suggested 1/16" or smaller Ball Mill, and/or #1 Spot Drill. That is what we recommend to our customers. Cheap and effective.

Use Pocket Routine (or MasterCam ART Module) for "filled" characters and Contour Routine for "line" characters.

To Program "filled" characters, use a Ball Mill in your CAM system and set your Step-Over or Scallop Height to achieve desired "Effect".

When doing "line" characters set Cutter Center Line ON and leave CUTCOM (D) at Zero in your machine. Spot Drill /or/ Engraving tools work best here.

There is already a lot of good advice here, just my .02C worth.

Kuyohtay
HARDINGE Inc.

[metalrulz]

Generally i use a conical engraving tool. .005"-.007" deep. with a small step over in a pocketing routine. In the past i've used a .093 ball but it just doesnt cut as nice. This is were i get them from. http://www1.mscdirect.com/CGI/NNPDFF...9596&PMCTLG=00

[lannyn]

I have had good luck using old carbide circuit board drills. I usually discard the drill portion and then grind a flat using my carbide wheel. I use a magnifyer head piece to get a good close look at the tip. I have thousands of these bits because I used to be in that business. If you want some send me a message and I will be glad to share.
Lanny

[PRADEEP R.KHARE]

Hay use h.s.s./carbide round to fit in machine collet chuck normal is 6.0 mm or 1/4"
grind some length to a cone of 30deg. to 20 deg.to match the Ø like pencil then a length to 1/2 Ø ie 3.0mm or 1/8"(longer than the depth of engraving) releve cone by grinding to create tool form till the half ground edge.(good finish required without any burning of tool material) now Hold the tool on Ø in collet of machine spindle.
& start using the same with good cutting parametres like drilling/milling.THIS IS KNOWN AS SINGLE LIP ENGRAVING TOOL)
T!!!!!!!!R!!!!!!!!!!Y!!!!!!!! NOW.
THANK YOU
PRADEEP R. KHARE
INDIA

[whayes]

It's best to use a v-bit cutter or a ball end mill. The level of the surface being engraved must be flat for the text to come out clean looking. If it isn't the text will be deeper in some areas than others. I always cut the surface to be engraved before actually engraving. That way I'm sure the text will look excellent. Because your only cutting at a very small diameter you should run the cutter at maximum speed. 20000 RPM is not to fast. I built a CNC router from scratch and have made lots of signs for people as well as contoured guitar bodies. Hope this helps you out
Willy