Keyway cutting in 316L shaft with CNC Mill

[GthomasRazorback67]

I really could use some tips on cutting keyways from 3/8 up to 7/8 in 316L shaft with a 50 taper CNC Monarch mill. It seems like I always end up making multiple shallow rough cuts to make my carbide end mills last. I would like to do 1 pass rough leaving .010" all around and make 1 finish pass, then chamfer of course. I am using NexGen coated end mills, stub length in ER collet holders. I use 2 of the same end mills, when my rougher gives up I move the finisher to the rough position and tool up a new finisher. Would I be better off using a roughing end mill for slottting? I have only used a roughing end mill for side milling applications. I do have coolant through spindles also. Would solid end mill holders using Weldon shank end mills be better? Right now I have more questions than answers so any advice would be greatly appreciated.

 

[MillGuy88]

I like to ramp down into the keyway in what I have heard others call a racetrack toolpath. I also use seperate tools for roughing and finishing. The tool manufacturer should tell you what the maximum ramp angle is for a specific tool as well as recommended speeds and feeds for specific materials to get the most out of your tool. I would be careful of your tool pulling out using ER collets. I like to rough with indexable tooling whenever I can.

When I was an apprentice, the rule of thumb was 1/2 the tool dia. for full slotting DOC with an end mill, and 1-1/2 tool dia. for full slotting DOC with a roughing end mill. Now a days there's videos of endmills doing insane full slotting DOC's without even chattering. Just depends if the tool and set-up can handle it I guess.

I use a macro program I created for keyways. Just input my variables like keyway length, width, depth, shaft dia., tool dia. etc. and the machine does the rest for me, It even spits out a measurement across the shaft that I'm aiming for. I have different macros for closed and open ended keyways.

 

[guythatbrews]

You'll get better feedback if you give more details. Such as:

1.Exact end mill
2.Feeds and speeds you've tried.
3.The failure mode you are seeing. Chipping, wear, or something else.
4. Open end or blind keyway?
5. Describe the cutter in the cut. Is there chatter? Loud, bad noises.

Chip recutting is a big issue with what you are doing. You'll see immediate improvement if you eliminate that. I expect your coolant isn't strong enough to remove the roughing chips. Is it?

 

[GthomasRazorback67]

Thank you!

 

[Mtndew]

stub length in ER collet holders

The end mill that roughs the keyways should be in a side lock holder if you go full depth otherwise the end mill will pull out.
Also that end mill should have a decent corner radius.
Could easily go full depth, but sometimes it's faster to either take depth cuts or ramp.
Finish end mill should be at least a 5 or 7 flute for efficiency if doing a large quantity.
You don't need a rougher, but it won't hurt to use one.

These end mills from PCT with the H5008 Exxtral Silver coating I've found to be amazing in stainless steel.

https://webshop.pct-imc.com/catalogue/product/1976151