Ramp parameters for fine text engraving in aluminum

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

Post Reply
Posts: 1
Joined: Fri Aug 07, 2020 2:41 pm

Ramp parameters for fine text engraving in aluminum

Post by nateflanigan »

Hello, I'm testing out engraving some pretty fine text in anodized aluminum. The text is 2.7mm-1.7mm high, I'm using an Amana 0.005" 30 deg v bit. I've experimented with both pocket toolpaths for true type fonts and contour for single line fonts. Depth of cut is 0.05mm. Generally I've been getting acceptable results, could be better, I was wondering if I should be ramping into these cuts. Since the lines are so short and the engraving is being done in one pass I wasn't sure if there was a point to ramping, but would of course like to get the best results possible.

Any other advice on how to optimize these kinds of cuts would be welcome. I'm using an sd100, I've been following the tool's datasheet, lowest setting on the router (dewalt 611) and a feed rate of 50 ipm.
https://www.amanatool.com/pub/media/pro ... art-v3.pdf

Here's an example.


Posts: 600
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA

Re: Ramp parameters for fine text engraving in aluminum

Post by Rando »

Your cutting parameters seem within what they recommend, if on the slow side.

As for ramping, I'd say "no". Terminology-wise, ramping, which occurs at an angle, is different from plunging, done vertically. In work like you've shown, variation in surface height could cause the entry location to change in a ramp, where it wouldn't in a vertical plunge.

But maybe more importantly, I find it interesting you're running at the LOWEST speed setting. If you consider that we're talking carbide cutting into aluminum, which want an SFM in the 900-1200 range, that 0.005" bit really needs something like 30K+ RPM to be cutting properly. I've had good luck in the 18-20K RPM range. Too slow and it dulls the bit too quickly; too fast and the aluminum starts to weld itself onto the cutting edge, aka "built-up edge". This happens the same on 1" endmills as it does only 0.005" engraving bits.

I've had really good luck engraving with a spring-loaded system that I got on eBay. Suspiciously expensive, it has proven itself in many ways:

* Fully adjustable tension for working with soft and hard materials.
* Bits don't break nearly as often because the entry is softer
* the cheapest split-shank engraving bits are the ones that fit.

The ONLY problem I've had with them is that you have to remember to grease them so the bit slides smoothly...and to keep the grease OFF any delicate surfaces you might be engraving, say like a glass bead-blasted surface that's already technically "clean".

Here's a link to the one I use. We've even done 0.020" deep engraving into stainless. I tend to like the 15-degee bits over the 30 or 60, since the line width is less affected by surface height variations across the part. Sometimes even just a few thousandths is enough to make it visibly different.

https://www.ebay.com/itm/Spring-Loaded- ... SwJD5d1iLJ

There are of course the American-made really nice ones, but they only take their own proprietary bits, which are of course more expensive.

I've tried the spring-loaded diamond-tipped engraving bits as well. They're very sensitive to coming down too hard, and accelerating from a stop too fast; they diamonds seemed to break off far more easily than I thought reasonable. Also, and especially on anodized surfaces like you're doing, the diamond drag engraving bits crack and fracture the oxide surface, making the result not nearly as well-formed.


ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply