Might be a dumb question, but...

[kreativjustin]

Hey everyone, so I'm a tool room CNC programmer. I was running a part the other day out of 4140 with a carbide rougher (link below), and I was told that I'm babying the cutter.

I was doing slotting, so 100% width of the tool, and was doing .100" per pass, and was creeping around 3IPM. Here's where it gets interesting.. I went back and checked the Feeds n Speeds (link below) and it recommends 1x DIA and 1x WOC to cut at 330SFM and .0016ipt

That converted out to doing a 1/2 woc, 1/2 doc, spinning 2521rpm, feeding at 16.1345ipm

Is it just me, or does it sound like that cutter is going to break? I'm not doing Trochoidal cutting, just a straight linear feed line.

I'm not used to machining at that aggression, but I need to make my tools last longer and get the job done at a more reasonable time.


1/2 4fl carbider rougher 1.25LOC

tool: Guhring.com: RF100 VA/NF standard length variable helix roughing-finishing ENDMILLs for stainless steels - Series 3081

speeds n feeds: http://www.guhring.com/Documents/Tec...n=080417012615

Similar Threads:

• Need Help!- Maybe a dumb question :(
• Maybe a Dumb Question But
• Dumb question, but not so dumb??
• Dumb Question
• dumb question

[awerby]

Was that recommendation specifically for a slotting cut? When the tool is engaged on both sides, it's much more stressful on the tool; usually you'd slow down by at least half compared to a normal pass where the tool is only cutting on one side. Also, speed/feed recommendations are usually calculated based on an extremely rigid and powerful machine. If yours is lacking in those respects, you'll need to slow down.

[hfjbuis]

I'm not used to machining at that aggression, but I need to make my tools last longer and get the job done at a more reasonable time

You have to cut, not rub.

Just some thoughts,

Cut as deep as possible to use as much length of the cutter. This way you use and wear the "whole" tool, not just the tip.
For production run's it may be profitable to find out what the machining limits are by some experimenting and this will break some cutters and work pieces.

If your machine and setup is rigid, the recommended (min) speed and feeds are a good starting point.

Roughing cutters are designed to go very fast and to leave a rough finish.

Prevent milling the just made chips. This will ruin the finish and wear the cutter.

[the_gentlegiant]

Your numbers are correct according to the literature you linked to, (at full width and depth, not 1/2) though you'll never get that cutter with 1 1/4 LOC to do anything close to that. 1 1/4" LOC means the cutter is likely sticking out of the tool holder almost 1 1/2". Way too much stick out for those F & S. (It would chatter like mad.) If you had 5/8LOC then yes I think you could approach those numbers. That is if your machine is stiff enough, and you're running fully annealed 4140 at around 187 BRH.

I can't even come up with a scenario with that cutter at 1 X depth and slotting. Your half and half idea is doable at say 2024rpm and 10-11ipm. Try working your way up to that for starters.

Even though that looks like a sweet cutter, you might consider 3 flute end mills for your slotting needs in the future. Even with the long stick out you have, a 3 flute could approach or beat those numbers you found for your rougher. I sort of gave up on roughers a few years ago. I believe there are better ways to skin that cat.

Dave

[kreativjustin]

Thank you for your comments. It seemed like it was far too aggressive. I have a Fadal 2016VMC with 10k Spindle

[liyary]

Your numbers are correct according to the literature you linked to, (at full width and depth, not 1/2) though you'll never get that cutter with 1 1/4 LOC to do anything close to that. 1 1/4" LOC means the cutter is likely sticking out of the tool holder almo my ip birthday wishes tneb st 1 1/2". Way too much stick out for those F & S. (It would chatter like mad.) If you had 5/8LOC then yes I think you could approach those numbers. That is if your machine is stiff enough, and you're running fully annealed 4140 at around 187 BRH.

I can't even come up with a scenario with that cutter at 1 X depth and slotting. Your half and half idea is doable at say 2024rpm and 10-11ipm. Try working your way up to that for starters.

Even though that looks like a sweet cutter, you might consider 3 flute end mills for your slotting needs in the future. Even with the long stick out you have, a 3 flute could approach or beat those numbers you found for your rougher. I sort of gave up on roughers a few years ago. I believe there are better ways to skin that cat.

Dave

I was doing slotting, so 100% width of the tool, and was doing .100" per pass, and was creeping around 3IPM. Here's where it gets interesting.. I went back and checked the Feeds n Speeds (link below) and it recommends 1x DIA and 1x WOC to cut at 330SFM and .0016ipt