My smallest engraving attempt

[Michael Simpson Virgina]

This is in a bar of Aluminum. Shown here next to a dime. This is done with a 1/4 vbit.

I cant really get the detail I want until I get my 1/4 to 1/8 bit adapter.

the o on robotics is about .01" high. They are engraved .003 into the suraface. While its no where near the acuracy and size of my laser. It is in metal which I can not do with my laser.


Question.

At this size should I be using higher RPM. This is at about 12,000 and at 10ipm. I have not tried other speeds as it seems pointless until I can use one of my smaller bits.

[Jim Underwood]

Looks like you've got a little "mushing" of the material going on. This can happen if you don't have proper chip loading in aluminum. It's a lot more fussy than wood. You have a narrower range of RPM/IPM choices in AL.

Of course I have no idea the state of your v-bit or whether it has the proper clearance angles either... I had one that had been sharpened so much that the cutting edges were ground past each other at the tip, and the sharpening service wouldn't grind any more clearance... So, it made a fuzzy cut... It was just a cheap bit so I threw it away and bought a couple more.

[Michael Simpson Virgina]

So if you get this mushing do you speed up the router or slow it down? Speed up the feed rate or slow it down?

[Dan Hintz]

You also need to be extremely sharp... you have two choices, slice the material away in a chip or push it around (as seen here).

[Wil Lambert]

So if you get this mushing do you speed up the router or slow it down? Speed up the feed rate or slow it down?

I think the problem you will get is the if you are using a router for a spindle you will never get a proper chipload on the cutter.

Formulas.

Chip Load = IPM/(RPM* # of Flute)
IPM = RPM * # of Flute * Chip Load
RPM = 3.82 * SFM/ Cutter Diameter

Approx SFM for aluminum starts at about 400. You have an effective cutter diameter of .006". This relates to and unthinkable 254666 RPM. If this RPM was possible you would have to feed it at about 20 IPM.

Now for what you are running. 12000 RPM at 10 IPM is about a .0008 chip load. You need about a .006- .008 load. This will relate to 96 IMP. You will never be able to accurately engrave at that speed. Running the tool at about 1300 RPM will yield a good chip load. This should prevent mushing as long as the cutter if sharp.

All of these figures assume that the Vbit is a single flute tool.

I have included a Speed and Feed calculator I wrote to help with this process.

Good luck,
Wil

[Michael Simpson Virgina]

I am working on a new cnc now. IT should be done in a couple of weeks. Roughly the same design but will have a Fordom TX. I should be able to get much lower RPM. I was thinking of adding an attachement to this cnc but I need to do a new one in order to document and create the instructions anyway.

[Jim Underwood]

Sounds like Wil has it going on.

I have had no success in milling aluminum, although my machine will handle it, I've not got a good fixturing table. We bought the waffle style table, and thought we were getting a grid style...

If you're making larger cuts in AL, you'll need to bolt it to the fixture because vacuum won't hold it. DAMHIKT!
Also, if you get very large, you'll need some kind of oil mister to keep it lubricated as you cut. Gets kinda messy...

[Michael Simpson Virgina]

Honastly all I realy wanted to do was to create some very small marks.

[Wil Lambert]

Jim,

Thanks for the compliment. My full time job is managing and programming for a mold shop. I work with 3 and 5 axis machines everyday.

Michael,

You did a good job on the engraving. More than I would have tried on my router. At work I engrave with cutters down to .005" in hardened steel. Never would I try this or even aluminum on my Techno router.

[Jim Underwood]

Jim,

Thanks for the compliment. My full time job is managing and programming for a mold shop. I work with 3 and 5 axis machines everyday.

Ok... Now I'm green with envy. I'd like to use more of the capabilities of our 3 axis router, but cabinet production takes precedence. ...and to have a 4th and/or 5th axis would be toooooo cool.

Well Michael, you'll need to play with those feed speeds and RPMs in order to get a good cut in AL. Having not done it on that small scale, I'm not sure what to tell you. In the end, it's trial and error. "Whatever works" as they say. Essentially the process is to get an acceptable starting point and then tweak feeds and RPM from there.

[Gerald Wubs]

Right you are Dan, While chip loads are important, what matters is whether you are CUTTING material. This requires "keen" sharp cutters, with adequate clearance. In fact too high a feed rate for a given spindle RPM can exceed the clearance of the cutter and make it push the material out of the cut like the picture.

[Hans-Joerg Mueller]

Using the special single lip carbide engraving cutters for this type of work would be a good start.