[MFchief]

Hi All,

I'm looking for recommendations for a tool bit for some simple engraving, such as a small brass nameplate, etc. I have no experience with engraving, except that today I did a 1 X 2 inch brass plate using a simple 3/8" 60 degree Vee cutter and the Mach3 Write Wizard. It seemed to come out fine, but I would think there would be better cutter choices.

I don't have a speeder, so I am trying to use the 5K spindle speed on my 1100. Should I look for a cutter with a tip radius or a straight Vee? If a radius, what might be appropriate for letters approximately .2" - .3" in height? A lot if the cheaper cutters I see on eBay appear to have a "D" bit design, would these need a higher rpm than my spindle?

Thanks for any help you might offer.
Terry

[TXFred]

I used a D profile cutter, 15 degree angle, with a 0.020" tip. This is in my Tormach 1100.

I don't remember the brand. I ordered it from MSC.

It works just fine, although I'm sure it would be faster if I had the speeder, a second spindle, or a 770.

Frederic

[twocik]

I'm using a Melin .125 mill/drill and works great for what I need. However it's really slow if you're running a 1100 without a speeder.

Enco - Guaranteed Lowest Prices on Machinery, Measuring Tools, Cutting Tools and Shop Supplies



TXFred - I'd like to see what you're using, have any pics up ?

[philbur]

A normal text height to line width ratio is 7:1. So with 0.2 to 0.3 text height you have a text width of 0.030" to 0.040. In my opinion 5,000 rpm is to slow to run a conventional end-mill at that diameter so the best is still the single lip conical engraving cutter, 60 degree for max strength. A 60 degree conical engraving cutter with a 0.010" tip would need a depth of cut of about 0.016" to give you a 0.03" text line width. To check the calcs you have to do some Trig.

Feed per rev. is best calculated as a % of the tip diameter and should always be less than 50%, it's kinda obvious why. I think 10% is a good starting number. Do a test letter and then look at the finish. You don't want the cutter moving forward faster than the relief angle is backing off if you understand what I mean.

I'm no expert but I have wrestled quite a bit with issues related to engraving small text. Judging by how much you can find on the net with respect to the actual hard facts it's probably on a power with witchcraft.

Phil

[rowbare]

Have you looked in to diamond drag engraving? Maybe that would meet your needs.

You can get diamond drag engraver bits for about $10 on eBay. I have purchased from brucediamondcorporation-2008 and was very satisfied with the product and service. If you search there for "drag engraver" you will find a couple of people who sell spring loaded holders. They are pretty simple to make if you have access to a lathe or do some mill as lathe stuff. Here is a link to how one guy built his: Diamond drag engraver | RoboCNC.nl

bob

[300sniper]

i've been using these for engraving stainless: Single Flute Half Round End Mills - Engraving Cutters | MSCDirect.com

using my 4500 rpm spindle, it's painfully slow. i run them at 4500 rpm and 2.5 ipm and .003" doc to a finish depth of .010". this is what i came up with from experimentation. any faster or deeper and i break the fragile tip. i really want to get an auxiliary spindle but i am not sure what one to get.


this is using the "complex" font in the write wizard:

[shred]

If you have a surface grinder or the like, grind up some pyramid bits on broken carbide shanks: Making Pyramid Engraving bits
I made one as an expedient on a weekend, but like it so much I probably won't be buying any more of the single-lip engraving cutters.

The other thing is you will want to do if you haven't is find some single-stroke fonts, as Windows fonts are all outline fonts and don't engrave very well at small sizes.

[MFchief]

All,

Thanks guys for the great info! it's all good stuff to get me started, looks like the bit I referred to as a "D" bit is what most folks call a conical. Those are pretty cheap on eBay, so I going to grab a few to experiment, also saw the diamond drag bits, so I think I will make a tool as shown in the great link and try that also. I like that idea because of the stopped spindle, so no RPM issues.

I also, amazingly, have some broken carbide bits, and a surface grinder, so I'm going to experiment with home made bits as well.

One follow up question for Shred, is the Mach3 Write Wizard using windows fonts, and is it possible to add fonts to the wizard?

Really appreciate all the advise, especially those who went to the trouble to add pics and links.
Terry

[shred]

All,
One follow up question for Shred, is the Mach3 Write Wizard using windows fonts, and is it possible to add fonts to the wizard?
Terry

IIRC the Write Wizard uses it's own fonts (so they are OK for engraving), but there are some single-stroke Windows fonts around that people have made for use with CAD programs. I don't have a link handy, but some Google-Fu for single-stroke fonts and windows should turn up something.

[MFchief]

Shred, thanks for the reply, and the info. I'll get out my google horse and go looking.
Terry

[philbur]

the key search phrase is - single line fonts

Phil

[magma-joe]

2L Spring loaded engravers are the hot ticket. Since they are spring loaded the surface does not have to be flat and they engrave at 15 to 20 IPM at 2000 to 3000 rpm. I started to buy a a spindle speeder and found the 2L which has worked great.


Spring Loaded Engraving Tools engrave flat and uneven surfaces

[ame=http://www.youtube.com/watch?v=RYLtL1R440E]Spring Loaded Engraving Tool for CNC Machine Engraving - YouTube[/ame]

Magma-joe

[twocik]

Nice !! Few questions for you...

Since it's spring loaded, I'm guessing the depth always comes out the same no matter how much you plunge the cutter (that's until you've reached the end of the spring). Or am I wrong ?


How are you getting such high IPM with less rpms... ? I mean I can only get like 1 - 3 IPM at 5140rpms before I start to see scalloping and I'm using a 2 FL flat topped mill/drill. I'm not complaining it works great, but I would love the speeds you're seeing without having to stop and load a big clunky speeder.

[VaderSpade]

Feed rate, spring strength, and multiple passes control depth. Because of the spring you can set your plunge rate very fast, which cuts you overall time dramatically.

Watch that video, and then check out others by the 2L company.

[MFchief]

magma-joe,

That is definetly a cool tool! I especially like that it can handle curved surfaces without having to go to a 4th axis.

Unfortunately, it's a little pricey for my once or twice a year engaving needs....
Terry

[Bob La Londe]

For quick and dirty brass I just use a spring loaded carbide drag engraver. I bought fancy tips and diamond tips, but one day I needed something done and those were all broken so I just chucked a broken carbide end mill in my lathe and put a grinding wheel on a rotary tool in the tool post and made a conical point. The one in this video has engraved about 60 plates like this one and has not needed to be sharpened.

It is not a "smooth" finish, but it looks good.

[ame=http://www.youtube.com/watch?v=MiVmrCznntE]CNC Engraving a Brass Plate - YouTube[/ame]

I have also used it to engrave my name on the side of impact sockets when I was testing to see what it would do. On hard steel like that it leavesa nice mark, but does feel smooth.

[magma-joe]

The 2l is pricey but compared to a speeder it is a deal. Attached is 2 charts from 2L for RPMS and feed rates for different materials using a RIGID TOOL and then the 2L . It also explains how the tool works.

Speeds and Feeds for Engraving Tools and Endmills

Magma-joe

[shred]

I tried a tool like the 2L but had trouble with it 'drilling in' on slower moves. What do you do to get around that?

[philbur]

Since it's spring loaded, I'm guessing the depth always comes out the same no matter how much you plunge the cutter (that's until you've reached the end of the spring). Or am I wrong ?

The video says the depth is controlled by the feed rate, which makes sense.

How are you getting such high IPM with less rpms... ? I mean I can only get like 1 - 3 IPM at 5140rpms before I start to see scalloping and I'm using a 2 FL flat topped mill/drill. I'm not complaining it works great, but I would love the speeds you're seeing without having to stop and load a big clunky speeder.

+ 1. I don't understand how they can have a feed rate that gives a chip load per tooth that is nominally equal to the diameter of the tool at the tip. Seems to me it would then be equivalent to a none rotating tool. It's not clear in the video that the tool is actually moving at 25 inches per minute .

Phil

[philbur]

I tried a tool like the 2L but had trouble with it 'drilling in' on slower moves. What do you do to get around that?

As the feed rate dictates the depth of cut I guess you possibly need gcode based on constant velocity mode.

Phil