Aluminum Engraving Job

[Brady Watson]

AJ,
Yes - HSS does cut AL better than carbide. It also seems to have less harmonics than carbide because it is not as dense. When I need to do thicker AL projects, I use HSS end mills from OSG. I believe the helix angle is more aggressive on the HSS cutters for AL to get the chips up & out faster than a standard end mill grind.

HSD RPM - It depends on how low your VFD is programmed. The V1000 is programmed to run 5,000 RPM as the lowest limit. In reality, you won't have enough torque to do any meaningful work below 8,000. The motors are wound to be routers...not milling machines - so you may have to increase move speed to get the right chipload to match the higher RPM...or deal with light chiploads.

-B

[Don Chandler]

Originally Posted by Ajcoholic

When you guys machine aluminum, why not purchase metal working cutters? (vs using cutters designed for cutting wood and composites)

I do metal work as a hobby. I purchase special end mills strictly for aluminum (they are HSS) that cut amazing. I dont know what it is about the geometry of the cutter - they look the same to my eye as all my other end mills for steel - but man, they certainly work 100% better when cutting any aluminum alloy, or raw aluminum.

ALso, how low an rpm can the HSD spindles be run?

AJC

You can also buy router bits designed for aluminum. I use them with my PC router on the SB and they work well. here is a pic of the running board plates I made for my 49 Ford truck.

[Brady Watson]

Originally Posted by donchandler

You can also buy router bits designed for aluminum. I use them with my PC router on the SB and they work well. here is a pic of the running board plates I made for my 49 Ford truck.

Nice running boards, Don.

The spiral-O bits they make for routing AL don't do such a hot job when you get into machining thick AL bar or need to do a pocket and want a clean bottom. The 2-fl end mills seem to give a better result with less deflection.

-B

[Joshua Ciaramitaro]

Originally Posted by bradywatson

Pull your speed down to .7 on XY and use a coolant. I like rubbing or denatured alky. Don't over-do it on the coolant. No dust collection if you use the alky(!). Increase depth of cut to .04-.06 per pass - only if you have a spindle. If you can get away with a 3/8" cutter, or larger, do it as there will be less tool deflection and less swirls at the bottom surface...plus less deflection at direction changes. Looks like the bit walked on the 1st pass of the lower right stroke of the letter 'A'.

The alloy you are ultimately going to be cutting, not the scrap/test piece, is what you need to focus on.

-B

Well I attempted to run with these settings today and did not have proper material hold down so it trashed my sample and bit. I am going to decrease the pass cut depth which seemed to cause the problem. I also have some different "engraving bits" and was wondering if these would work and how to set them up in V Carve as a Toolpath would this be considered an endmill? The bit has a .030 TIP with a 30 Degree Angle and 1/4" SHK DIA with a 2 OAL.Thanks again for all the help everyone!

[Joshua Ciaramitaro]

http://www.onsrud.com/product/Item/m...FB010?q=66-320

This is a bit I am considering ordering for this job...

[Joshua Ciaramitaro]

Originally Posted by bradywatson

Nice running boards, Don.

The spiral-O bits they make for routing AL don't do such a hot job when you get into machining thick AL bar or need to do a pocket and want a clean bottom. The 2-fl end mills seem to give a better result with less deflection.

-B

Well after many headaches, broken bits and well COUNTLESS hours I have been able to produce the majority of this job so far. I am getting nervous when it comes to engraving this thick aluminum with a .0625" bit which I am sure will snap the bit (Which is why I have about 10 backups) So far though so good thank you all for the advice thus far I will be sure to post pictures of some of the completed engravings once I get closer to finish. Thanks again everyone for the help this community is incredible!

[Joe Crumley]

There are O so many trophy engraving shops that are set up to do just this kind of work. Their equipment is designed for this kind of work. I know what I'd do. Give this job to them and take home some good money. I'm not into misery.

Joe Crumley

[Joshua Ciaramitaro]

Originally Posted by joe

There are O so many trophy engraving shops that are set up to do just this kind of work. Their equipment is designed for this kind of work. I know what I'd do. Give this job to them and take home some good money. I'm not into misery.

Joe Crumley

Whole heartily agree!! Now if only I could convince the boss man.....

[Brady Watson]

Josh - Engraving is very different from V-carving, even though PartWorks calls V-carving a V-carve/Engraving toolpath.

Generally speaking within the context of your application, engraving is typically very shallow, with a max depth of maybe .08" deep. The bit you show in your pic, is suited to shallow centerline/single stroke engraving only using an 'ON' profile toolpath. If you push it deeper than that it will snap.

V-carving is typically much deeper, and v-carving in AL is tricky because of the geometry of the bit itself. V-bits don't really cut on the very tip, they drag, so if you go at it like wood, you'll really be hammering that bit. It is not impossible to v-carve AL, but you really have to be conservative with stepdowns and plan your cuts...and even think outside the box a little.

The examples that you show on page 1 of this thread appear to be pocketed out using a pocketing toolpath strategy. What happened to this? It will be the least amount of aggrivation compared to v-carving. Shallow engraving would be the easiest with the engraving bit you show - although I am partial to Micro100 for engraving tools as they are really tough, have shorter flute lengths and hold up really well in non-ferrous metals.

-B

[Joshua Ciaramitaro]

Originally Posted by bradywatson

Josh - Engraving is very different from V-carving, even though PartWorks calls V-carving a V-carve/Engraving toolpath.

Generally speaking within the context of your application, engraving is typically very shallow, with a max depth of maybe .08" deep. The bit you show in your pic, is suited to shallow centerline/single stroke engraving only using an 'ON' profile toolpath. If you push it deeper than that it will snap.

V-carving is typically much deeper, and v-carving in AL is tricky because of the geometry of the bit itself. V-bits don't really cut on the very tip, they drag, so if you go at it like wood, you'll really be hammering that bit. It is not impossible to v-carve AL, but you really have to be conservative with stepdowns and plan your cuts...and even think outside the box a little.

The examples that you show on page 1 of this thread appear to be pocketed out using a pocketing toolpath strategy. What happened to this? It will be the least amount of aggrivation compared to v-carving. Shallow engraving would be the easiest with the engraving bit you show - although I am partial to Micro100 for engraving tools as they are really tough, have shorter flute lengths and hold up really well in non-ferrous metals.

-B

Hey Brady,

Thank you for the advice your wisdom is much appreciated. I am for this job actually creating a pocket with a .25" Single Flute Upcut Sprial bit. The finish has been incredibly well and so has the running it through the material. It was a process to determine the correct depth of each pass and also a good feed rate but now that is dialed in, this job is going smooth. I do agree that v carving was not the correct way to begin this production which is why I have switched gears and gone with pocketing. (A learning curve) I am getting more and more comfortable with everything considering I have no background in any type of routing, milling or anything that has to do with a saw or cutting. So to say the least this is a whole new world and language for me. Once again I appreciate all the tips and will post up pics of some finished pieces soon!