Alluminium engraving????

[contour]

What cutters do you use for engraving alluminium,i generally just use standard ballnose cutters,0.5mm-1mm range but they are limited to depth of cut and feedrate, does anyone have any better ideas to increase tool life and increase productivity.

[Superman]

What depth ?
Stick form letters ?


if part marking.
D bit single flute, 50 deg included angle, point dia 0.1/0.3RPM = fastest
Z plunge rate =200mm/min
XY feedrate =300mm/min
Cutting Depth= 0.1mm deep

the broarder the angle - the stronger the point, but also the less detail on deeper engraving
check by rotating the tip on a projector, back of the cutter must not come outside the cutting edge

[contour]

Those speeds/feeds are just about what i am running with the 0.4mm ballnose,the d-bits dont give a good enough finish because they go to a point, a more broader inside surface area is needed visually. Some lettering needs to be backfilled with paint and the dbit type for some reason doesnt look that good when painted.

[TORISKOGEN]

What cutters do you use for engraving alluminium,i generally just use standard ballnose cutters,0.5mm-1mm range but they are limited to depth of cut and feedrate, does anyone have any better ideas to increase tool life and increase productivity.

for engraving i use highspeed senterdrills cause they cost allmost nothing and i can use bouth ends

[LeeWay]

I actually grind my own from a drill bit. I have some pointed and some with a small flat bottom. I run them at 6600 rpm with coolant and feed 150 IPM. Works great for me.

Before that I used mill drills. You can flatten those points out too.

[2dww]

I do a lot of Aluminum engraving. I use engraving bits from Harvey Tool Company. http://www.harveytool.com You can run your RPM as high as you can go. Feed about .003 per tooth chip load. For a good finish in 6061-T6 Alum use isopropanol alcohol
as a coolant. Softer the alum slower the rpm, and then use must use a coolant.

[Paulo E.]

As 2dww suggested, Harvey Tool has a wide array of engraving tools. Micro100 has some engraving tools as well.

My suggestion for the type of application you are looking for is to use an

engraving tool with no more than 40 deg included angle with a flat of .010


Depth .007 to .010

RPM 4500 - 18000

FEED 10.0 to 75.0

I know that as you can see there is a wide range of feeds and speeds. The reason I put that is because I dont know what kind of machine you have, collet system and speed limitations. I have a Haas VF1 and with a cat 40 system. I usually run it a 10.0 IPM and 4500 rpm. To tell you the truth even in running a production run, you wont see much difference in the engraving unless the engraving you are doing is quite a bit of engraving per part. If thats the case then you do need to optimize your Feed rate to what would be acceptable for your finish requirements. Dont be shy on the RPM and again the feed rate is something you have to decide what is the acceptable finish criteria.

[diecutter]

Those speeds/feeds are just about what i am running with the 0.4mm ballnose,the d-bits dont give a good enough finish because they go to a point, a more broader inside surface area is needed visually. Some lettering needs to be backfilled with paint and the dbit type for some reason doesnt look that good when painted.

I use D bits, also called split point carbide cutters every day in tool steel. To get a flat bottom on the cut, simply "tip" the cutter. That is, using a ruby stone, hand stone down the point of the cutter with about a 5 degree side angle, a 10 degree back angle,and whatever width you desire. Very fine finishes are possible and the cutters are very easy to resharpen.