Milling deep into 6062 T6

Using my Storebro Combi-mill, (top spindle rpm 2500) - 1980s cnc mill

Just looking forward into situations I'm bound to find myself in....

For contour passes, I use 3 flute 10mm dia endmills (25mm usable cutting edge) full doc, 3mm stepover for roughing down, then to 0.2 on finishing passes. The finish has been very good. I could prob go double the stepover but haven't had the machine long enough to test it properly.

using 2D contour passes in fusion, I would like to know if its best to use a large dia endmill to rough the contour passes down. I wondering if I can get away with a 20mm dia ( 50mm long flute ) 35mm doc then go in with a 10mm dia for finishing passes.

As I understand it, going up in diameter but trying to keep the feed rate, DOC etc the same will result in a higher surface speed and spindle power. That may not be an issue depending on your machine if you ensure the chips are cleared successfully - that's what has cost me most cutters over the years. Air blast or high flow coolant is the best solution. Make sure you use uncoated cutters and ideally polished / honed at that. Max surface speed isn't usually limited by the cutter but by the machine spindle speed or spindle power.

Generally I use 10mm diameter carbide cutters or larger indexable tools. Bigger carbide cutters cost a lot more per crash! I often use my 50mm indexable shell mill with APMT / APGT inserts to the full 10mm DOC - these are often only used to take skim cuts but are in fact great for roughing.

The only time I use less than 10mm is when the slot or internal radius requires a smaller diameter cutter.

Thanks. The reason I say I'm thinking about using a 20mm dia cutter, is the doc. if I'm going 35mm in one pass, then tool deflection could be an issue ?. So I thought about using the 20mm endmill do take 95% of the material away, then go to a 10mm dia endmill to do the finishing passes at full depth. I have a 50mm shell mill. A bit nervous about doing anything else but surfacing with it.

The best place to get a rough idea of material removal rates, is to stick some figures into a speeds and feeds calculator (FS Wizard is free online, and good enough for most things).
Your approach sounds fine, you just need to make sure that your CAM can handle it (You need to tick the box for Rest Machining in Fusion).

And as Muzzer has mentioned, chip clearance is key to avoiding disasters in aluminium.

Quote:

---

Originally Posted by dudz

I have a 50mm shell mill. A bit nervous about doing anything else but surfacing with it.

---

Here's a 50mm shell mill doing 3D adaptive roughing. Safer / easier than using a long series carbide tool, which would otherwise be needed to reach the bottom of the stock.
https://www.youtube.com/watch?v=sSUmBLUvf9I

Deflection of a carbide cutter shouldn't be an issue, as they are designed to be used that way.
Here's an example of a long series cutter taking a good DOC. And showing the importance of good chip evacuation! making loads of chips in a corner with nowhere for them to go almost guarantees a breakage. The chips get "recut" and melt onto the tool.
https://www.youtube.com/watch?v=ypTLWvJlQ80&t=1s

Ok thanks, I get that, being its a long tool with sideways force. But if that was a 20mm or 25mm dia tool using compressed air, it more than likely wouldn't of snapped eh ? The shell mill was impressive in that video. But if the space was tight and you were forced to use an endmill, maybe a reduced neck endmill would be the go ? Speaking of which, I cannot find reduced neck endmills on aliexpress.

Yes, those reduced shank end mills are great for deep cuts where the surface finish needs to be good. The only engage with a limited portion of the total depth yet have a good reach.

I have used YuZe Tools on AliExpress (I dealt with Rickie Fang [email protected]) several times in the past for well priced, good quality cutters - end mills, thread mills, chamfers etc. It may be worth asking them if they do them. Previously I have bought them from Cutwel in the UK (for both steel and aluminium) when they were on offer at much reduced prices.
https://www.aliexpress.com/store/508...50ff4cadvh5NJK

Thanks. As regards to a 10mm endmill, having a reduced dia shank, would 9.2mm be about right ? or would it not be reduced enough ?

The YG-1 "extended neck" AluPower cutters have 9.2mm neck for a 10mm cutter. It doesn't need much reduction, as it's simply trying to avoid contact with the previous stepdown.

Here's the ones I got. These are usually £60 here in the UK but I wouldn't ever pay that much. Cutwel do some nice reductions from time to time but I don't recall what I paid. Page 13 of this flier, if the link works:
https://s3-eu-west-1.amazonaws.com/c...-hpc-flyer.pdf

Nice, I have contacted Rickie Fang for endmills. Any recommendation for boring heads ?. I need something accurate for holes up to 80mm in dia

I got one of these boring head kits. Covers 8 - 320mm with the range of boring bars supplied. It doesn't do facing operations like a Wohlhaupter but you'd need to pay a fair bit more for one of those.

If you want a deep 80mm bore, you may want a smaller diameter head that would fit within that bore.
https://www.aliexpress.com/item/4000....4000551597026