[toothandnail]

Why are we breaking bits?

6061 T6, full flood coolant 5000 rpm
Bits .25" Dia / 1.75 Loc -Interstate and Hertel 2 flute 37dg HSS/HSS-Tin
Depth .05 / 10 ipm went to 7 ipm still breaks , chips are tiny
25% stepover
program run time 11 hours @10ipm

bits are losing their edges before breaking, cut is super smooth for the first5-6 hours, then it seems they loose an edge .

What do we need to change?
UPDATE

Thanks, for the replies!

Looks like we will be using a 3/8 bit for most of the roughing, that will cut the run time as well.

We were hoping to stay away from a tool change, as we need to run this overnight, more labor intensive operations during the day.

[txcncman]

As a starting point - Switch to carbide. SFM - 450. RPM 6876 for 0.250 Dia. 27.5 IPM for 2 flute. 0.2 axle DOC. 0.2 radial DOC.

[toothandnail]

We are maxed out at 5K rpm

[SCzEngrgGroup]

As a starting point - Switch to carbide. SFM - 450. RPM 6876 for 0.250 Dia. 27.5 IPM for 2 flute. 0.2 axle DOC. 0.2 radial DOC.

0.2" DOC/27.5 IPM with a 1.75" long 1/4" endmill? I don't think so. He wouldn't make it even one inch.

With such a long tool, you'll need to go VERY shallow, as the tool will be deflecting a LOT, which is certainly what's killing it. But you indicate it cuts fine for 5-6 hours, then the edges go dull, and the tool breaks. So why aren't you changing tools BEFORE they go dull, if it's working OK up to that point? 5-6 hours is probably pretty good life for a tool working under such difficult conditions. A dull edge will dramatically increase deflection. If you're really getting a good result for those first 5-6 hours, I would swap out the tool every 4 hours.

Overall, you'd be better off finding a way to do it with a larger diameter tool. And carbide is likely to help, as it's much stiffer. But, at the same time, it may well dull, or even break, much sooner, as it's so much more brittle, and much more easily damaged than HSS.

Regards,
Ray L.

[txcncman]

Actually I meant 0.1 axle DOC and 0.1 radial DOC. Sorry.

[txcncman]

For the carbide mentioned above with 5000 RPM maximum, change the feed to 20 IPM.

[SCzEngrgGroup]

Actually I meant 0.1 axle DOC and 0.1 radial DOC. Sorry.

Even that is very aggressive for such a looooong tool, and I assume he HAS to be cutting full-width a good portion of the time to clear the spaces between those bosses.

Regards,
Ray L.

[toothandnail]

update in OP

[mike sr1]

What is the actual depth of the cut in the part?
Is a cutter that long needed for your operation?

[jid2]

- What is the order of operations?
- Is that a single part, or a bunch of the same part?
- What is the spacing between the bosses?

[philbur]

Tiny chips would normally indicate to lower feed rate which could mean you are simply wearing out the cutting edge. If it cuts fine for the first 5 hours maybe you should experiment with a higher feed rate. Of course as Ray points out the tool length may be a limiting factor preventing higher feed rates. Best way to find out is try it.

Phil

[Runner4404spd]

break it up into two tools. use a shorter endmill do the top portion and get it done alot quicker, the switch to the long reach end mill and finish the bottom half.

or

use a drill bit and drill out the majority of the periferal material and then use and end mill to finish. again if you use two end mills then the shorter end mill can use more aggressive speeds and feeds and then only use the long for areas you can't reach and for finish passes.

option 2 doesn't seem elegant but working in a home shop its probably your best bet.

[tbaker2500]

Rules of thumb-
Use the biggest diameter tool you can.
Use the shortest tool you can. Those two let you:
Run the bit fairly hard, which keeps down rubbing.

But I would really consider switching to a carbide for your 1/4". I don't have any chipping issues, and the stiffness will give you a much better finish.

[MichaelHenry]

Though that looks like a fairly stiff chunk of aluminum, could part of the problem be due to the part overhang on the sides of the vises?

Whenever I attempt cuts on parts like that I get a lot of chatter, essentially all of it from the part vibrating while cutting away from the vise.

Perhaps 2 vises to hold the workpiece would help.

Mike

[Steve Seebold]

To cut between the webs, I would never use a linear move for that type of cut. I would develop a hole pattern and plunge the material out to ruff it, then make a program to finish it. I would probably make a program using 2 cutters, and I would throw the HSS stuff in the garbage and use only carbide.

[MetalZilla]

Try 3/8 3 Flute MicroGrain Carbide endmills from Fullerton Tool. I used them extensively in my RC parts business. Worked great!

[JohnToner]

Steve is absolutely right. Last summer I made an AR lower (on my knee mill). The material was 7075 and required much relatively deep pocketing. I rough drilled to remove as much metal as safely possible, then finished with 3 flute carbide end mills, minimum possible stick-out. No problems.

John

[toothandnail]

Thanks for the replies , we will have to learn the plunge cutting method you guys are doing, sounds like that would be MUCH faster as well.

So are you using s drill bit for the ruffing?

Haven't been here for a while , too much stuff needing done.

[Steve Seebold]

If you are going to plunge ruff a pocket, I would seill a hole the soze of your end mill first, then finish your plunge ruff with your end mill taking cuts about 35% of the diameter of your cutter.I.E 3/8 diameter cutter, .130 to .15 wide cut and feed down at 30 to 50 IPM debending on the depth of your cut.

Make your program by creating a drilling routine and use either G81 or G83, again depending on the depth of your pocket/slot.