Hi everyone!

I'm working on engraving an aluminum panel (about 1/8 thickness) with very fine detail lettering and I'm wondering what the proper procedures are for this.

Currently I'm using a 15degree V cut bit to a depth of 0.3mm (spindle speed is uncertain, but I am using the spindle from lumenlab in the upper quarter of its speed adjusters range). I've definitely discovered that feed rate can make or break the tip of the bit, but I can't seem to get a cut that minimizes the hanging burrs and I'm sure there must be some standard practice that I'm just not aware of yet.

Some ideas I have, but I'm not sure if they are good ones:
1) Do a cut with the V bit, then give a surface pass a greater angle V bit?

2) Multiple passes with the same bit?

3) Perhaps try to use a ball end bit?


Currently I've cleaned up the panel greatly just by rubbing it with steel wool, but I can see that many of the burrs were just bent back down in the groove that I'm trying to clean out.

Full set of images on flickr

Click to view attachment
** Yes the giant E was a mistake -- sometime EMC will show you your file, but not have it loaded **
Click to view attachment
Click to view attachment

All pointers are much appreciated!

Kurt

Hi Narwhal-
I'm just going to throw this out there, and this by no means may be the solution(s), but:
-severe burring like this can be indicative of a dull bit- that is, the bit ends up partially melting and parting the metal as much as cutting it..
-the aluminum alloy you are using is listed under "poor" or "fair" for machinability.
-It also could be that you have the wrong ratio of spindle speed to feed rate for the bit you are using..


Solving the first is easy- try out a new bit..

The second is relatively easy, if you bought your stock as "aluminum sheet" it is 9 out of 10 times going to be one of the 2000 or 3000 series aluminums- which aren't known for their machinability, but are known for their cheapness- this is the same stuff that aluminum foil is made from. Try using a sheet of either 6061 alloy (a general-purpose moderately high-strength alloy that machines well), or possibly something in the 5000 or 7000 series (other high-strength alloys). Onlinemetals.com has a decent and short guide for alloy selection..

The third is a little touchy... I've read all sorts of things about recommended feed rates for metals, and generally there seems to be no consensus for high-speed spindles. Clear and consistent information exists for low-speed multi-horsepower spindles, but, really, if you're running one of those you probably don't need a cheat sheet. Anyways, I'd suggest doing some test cuts at a slower feed-rate while maintaining your spindle speed, if it improves, then you have your answer. If not, try reducing the spindle speed as well...

And, if none of this helps (I have to admit there seems to be a bit of voodoo involved with getting the right ratios), you can always deburr the entire sheet with a belt sander....

All good bits of info Robin.

A few more details:

1) I believe I am using 6061, but I'll have to go over to the store to verify. There is an awesome metal store just a few blocks from my office call Industrial Metal Supply. I go check tomorrow.

2) The bits are brand spankin new, so if the bit is to blame its either:

a ) I have the wrong feed rate and ruined the bit too quickly (I can't go any faster with the micro, but I can go slower. The china spindle could use a bit more torque to really go slower)
b ) It's the fact that the bits are from china. (I certainly don't rule this out, at least I have a ton of them)

3) As it was milling everything I tried varying both the feed rate and the spindle speed within the ranges I have available, but nothing really resulted in a clear improvement. I just hope I don't need to go higher in the spindle speed. I guess my main step will be to slow down the feed rates in the file and try a few passes on ridiculously slow speeds.

What kind of bit are you using?

Does it look like either of these...



Does it look like something else?

I've heard the "half-round" or "single flute" cutters do a good job engraving, but don't really have enough experience with either of them to make that call myself.

Exactly. Except it's 15 degrees, so its very sharp.

Update: I checked in the store today to see which grade of aluminum I am using and it's 6061.

I have to plead a bit of ignorance as per engraving bits, but a ball-nose 2 flute end mill should have little trouble with 6061.....

The main problem is high spindle speed and a low feed rate. You can't do much about the feedrate.

I would set the spindle to its lowest speed that should be around 6 to 8K. Spray the work with some WD-40 and cut about 3 pases with the feedrate set to max. 12IPM?

3 pases at about .1MM and the last at .05mm.



Good luck

It seems to me that using a vibrating tumbler with glass beads might be a way of dealing with the burrs. Check out the vibrating tumbler that Brainchild put together. Link

I'd suggest you are going too fast, too. Try slowing it down a little bit, so you get good chip formation, rather than dust. Feeding too slow with a high spindle speed causes very, very fine cuts, and these can leave very fine wafers of metal behind, like you seem to be getting.

Another option might be to try a ball nose or other design of cutter?

I'd say add more flutes.

Thanks everyone. Your suggestions are appreciated. I tried again last weekend using some other tools with moderately better results (sorry I don't have images yet). The lines vary from perfect to almost exactly the same as the first panel.

I used a multi-flute (ie: more than 2) chamfer mill similar to the one in the posts above and it does work nicely if I do very light passes at 0.01mm depth each pass. Definitely time consuming and I need to turn all my paths into subroutines to automate the engraving process.

It seems that the surface height of the panel is very inconsistent which makes it hard to set zero. I've done some passes where its making visible grooves in one area and seems like its taking off atoms in another area (visible lettering, with an undetectable depth). I've seen some spring loaded engraver bits and think that would be an awesome idea if I had a spindle that could hold a 1/2" bit. I'm considering drilling and milling a surface to use as a vacuum table.

I found this image on a panel engravers website and it represent the kind of results I want to get. When I asked him nicely what kind of bit it was using in the image he both never responded and removed the image from his webpages.. it's a good thing I'm sneakier than that because I believe eventually someone will recognize what engraver this is.
Click to view attachment

If anyone can identify what's being used there I'd much appreciate it. I'm guessing its a diamond tip engraver which I may move to trying next, but my experience with diamond bits on aluminum is that they get clogged up quickly, but always produces a smooth surface.
Click to view attachment

I just came across this awesome site about engraving cutters. Great details there.

I really should get more scientific about this search for the perfect engraving. There are so many things to try.

There is no reason to use diamond tipped in fact I would think it would not work at all for AL. All the diamond tipped cutters I have seen have been used on vary hard steel and other super hard metals instead of grinding.

Your problem is melting the metal from having the heat build up in the bit and then the bit melts the metal. In normal cutting most of the heat is removed by the chip. If the chip load is too low the bit will heat up. The faster the feed rate the lower the cutter temp. It sounds strange but it is true.
The bit also rubs the work even if the cut has been made. This heats up the AL and the bit.

You could do water cooling but I just don't see the need.

You might look at what kind of bits this unit used.

http://www.youtube.com/watch?v=RZlI-rZ3TjE

IMO This looks remarkably similar to the engraving machine tip.

Click to view attachment

Can you post your g-codes so I can run some tests?

Sure.. good idea.

Main Text.ngc.zip is a section that I've parameterized and turned into a loop - should be pretty self explanatory.

Archive.zip contains all the text and line sections of the panel as individual files.

Finally sweet success.

I really didn't think a 90degree two flute would ever give good results because if I had to go to any great depth to get the bit to touch in all areas it would completely obliterate the center parts of letters like "A". In reality it does exactly that, but the results prove I'm on the right track. I'll have to move down from 90 degrees to 80 or 60 degrees, just not 15.

The results were perfect though, with no burrs at all, just clean cuts.

Here's what I found:

if multiple passes are needed, stepping down by somewhere between -0.05mm and -0.1mm is perfect. Anything less and you risk getting shadows to the letters because it requires so many passes and the metal may contract and expand during that time.

While I think my zero was decent, it didn't actually start cutting until about -0.2mm. At that time it was only cutting along the far outside edge of the panel and nothing else.

The inside area of the panel didn't get touched until I was at a depth of -0.35mm, so the panel surface varies by (probably) over ~0.15mm.

Pictures:
Click to view attachment
Click to view attachment
Click to view attachment

I don't know if this camera is being kind enough to the results. I think my cellphone took better shots before.

Nice! I really think you should be looking at something like this:


http://www.bitsbits.net/index.php?main_pag...514cb604ce5894e

How much do you have to slow down for that fine point tip to keep it from breaking?

The 2-flute flat tips that I'm now pursuing are a very popular search result for aluminum engraving. The ones like you show there seem to show up a lot on wax engraving. If you have one and run a test I'd love to see the results. Finer tips seem like a good thing for sure.

Also it just so happens that the flat faced 2-flute ones I'm using are dirt cheap in quantities of 10 from China via eBay. :-)

I painted a panel black then engraved it as a test run for getting the panels anodized.

The section lines were done in passes to see what works best. You can see from the images how the panel height changes.
Click to view attachment
Click to view attachment

I then decided why not go to the max depth of -0.38mm and do all the text in one pass. I still had to stop in in places and hold the panel up slightly to catch even deeper areas and occasionally press it downward to prevent deep letter cuts, but that was rare and fairly easy to deal with. I just released the clamps on one end of the sacrifice and lifted it.
Click to view attachment
Click to view attachment
Click to view attachment
Click to view attachment
Click to view attachment
Click to view attachment
Click to view attachment

As it was engraving, the chips were perfect, from about 1mm to a few mm in length, and I didn't use any cutting fluid at all.

Can't wait for the 60degree bits to arrive

Your results look great! Keep up the work, though it's making it even harder for me to wait for my micRo to show up O_o

Looking good...
FWIW, I've been known to use an (flat-bottomed end-cutting) end-mill to avoid the problem of varying line thickness with height... But I don't think you'd be able to get the fineness of detail you've managed to achieve. So, congratulations...

Did you tape the panel down with double sided mask?

This "pressing and pulling" business is not acceptable.

"Slowing down" is relative. If you start above the surface's highest point, and take small descending Z multiple passes at high speed, it is the same as taking bigger Z cuts at slower speeds.

Might not be such a bargain - you need to find the right tip. Why buy a $1000 machine then skimp $5 on the bit that actually does all the work?

I do the opposite. I buy cheap drills and expensive bits.

As for the depth issue, it's definite issues with the flatness of your base board/sacrifice material if you are clamping it properly, but it is more likely, from what you describe, that you are bowing the work material upwards with the clamps along the edge.

Try double sided tape as BC suggests, or, better still, get a vacuum holding system to suck it flat to the bed.

Also, do you need anything under the machine? You are engraving, so you are never going through the material entirely, are you? It's only use is to put the holding screws into, and if you get rid of those, you can ditch the board as well.

The reason I recommend the cheap bits is first and foremost because they worked excellent and second because they were cheap.

The vacuum holding system arrived yesterday. :-)

Umm, sorry to go OT, but what kind of keyboard is in this pic? Looks nice!

Standard Apple keyboard


Back OT = Vacuum table images which I can now share since I won the auction on ebay: