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

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

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

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.

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.

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.....

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".

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.

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?PMPAGE=631&PMITEM=00199596&PMCTLG=00

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

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

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

60 deg included angle engraving cutters work well for me. I am normally only doing single stroke engraving from a romanS font thay has been exploded and imported from Auto Cad. I am normally only going about .010-.015 deep.

Does anyone have a source for a spindle. High speed, 4000-25000 quiet, water cooled??? collet changing system, I have searched the web but with no luck. The diameter can be as large as 3.200" I will make the mount to suit the spindle. I saw a machine at the woodworkers show in Milw. WI and spoke to their rep. He was not at all interested in selling me a spindle unless it was $1200-1500.

How about omllat, that seems the best in spindle

Do you have a source?

You can get all the engraving tools you need from Engraveograph. I used these tools to engrave in Stainless steel during a production run. They are the guys that have been in the business for a very long time and have the experience that's required to get the best results in any kind of metal or application. They will work with you and steer you right because their reputation is on the line.

Really great Engravers made by Harvey Tool (http://www.harveytool.com/products/index.php?page_function=show_family&product_family=Engraving+Cutters&category_id=1)

I rather the 2 flute 60 degree from Harvey Tool while at work they buy the single flute conical blank from Melin Tool (http://www.endmill.com/).

thanks for all the replies
I did not know anything on engraving so I really appreciate all the help
if you have any more sudgestion or ideas I would really be interested,
for know i should go out and purchase some tools and try some engraving
thaks again:cheers: these drink is on me

I have used Ball Em to the 60deg spade shown in the links from Cutting molds to parts to prototyp stuff. there are allot of good thoughts here.

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. if you don't know the proper way to do it this is an issue. but other wise not a true statement.

Here is a few thinks from the last year and the Mirror plaque from my old show car from 10 years ago.

Also if you want some mastercam basics for engraving use my link in my sig and at the bottom of the page there is a button called Engraving.

I have used Ball Em to the 60deg spade shown in the links from Cutting molds to parts to prototyp stuff. there are allot of good thoughts here.

if you don't know the proper way to do it this is an issue. but other wise not a true statement.

Here is a few thinks from the last year and the Mirror plaque from my old show car from 10 years ago.

Also if you want some mastercam basics for engraving use my link in my sig and at the bottom of the page there is a button called Engraving.

X3 LOOKS NICE!!!!!!!!!

I scoped out the 4th Axis Engraving Video, and you make it look easy, and the Options, NICE!!!!!!!!!!!!:D

I have even used a #1 or#2 center drill in non-ferris metals. It cuts very nicely and with small depth of cut it will perform for a long time. I usally use this on lettering, although it will work in some countouring applications where hentracking design is wanted. My next choice is a small ball endmill for contour engraving. And of course the standard 1 flute engraving tool. Much care is needed in lettering with this. It will last far longer if a small radius is on the tip. Good luck. bradmancue

Tom, you any were near Crissair up there in AV? I was up there last sat doing some trainning as I see you are local.

hi again do you guys know if the engraving tools have a 3/8 shank thats because all I can fit on my mill are 3/8 diameter ,

X3 LOOKS NICE!!!!!!!!!

I scoped out the 4th Axis Engraving Video, and you make it look easy, and the Options, NICE!!!!!!!!!!!!:D

where do can you get this x3 videos

Under my Sig sir. the last link and then go to the bottom to the buttons.

We use a #1, or #0 center drill spinning as fast as you can with a feedrate of F20. and a depth of .005 to .010

thanks