Speed this up

[Sambo]

Material is 6061. Keep in mind that the tools in the feature I am focusing on have other purposes that I won't bother going into. I am using them to keep my tool count to 20. The feature is 1.25 dia. 2" deep through hole. Currently, drilling through with a 45/64 drill, then (this part needs to go faster) helical boring with a 3/4 rougher leaving .020 to clean up with a 3/4 finisher. Starting at center ... thinking I should bump up the default rough pitch from .08. S2000 F24. Any thoughts?

[DavidB]

Helical down at an angle instead of a depth.

Start with 3 degrees

[Guest]

I'd bump up the speed and feed too

 

I generally use 12,000 RPM with a feed of 85 IPM on something like that

[Colin Gilchrist]

+1 John

 

I'd go between 5000-12000 RPM (depends on what you've got at the machine, and about .01 per tooth per revolution.

[Ocean Lacky™]

why bother with the drill? just helix bore the whole thing.

[beej]

or drill with an OTM Holeshot drill at about 10 ipm it will be about .010-.015 undersize then finish with an endmill.

[Surface]

I agree with Ocean Lacky. Loose the drill. Speeds/feeds also seem a little too conservative, If it's a HSS 3-flute rougher, designed for aluminum, I'd start somewhere around 3300rpm (650sfm)and .01 FPT, adjusted for the centerline difference, comes out around 39ipm.

[Sambo]

Sorry, I guess defining what tool I'm using in more detail would have been more helpful. 3/4, fine tooth, 4 flute, TiCN coated, 3" LOC, NOT center cutting. Any time I have a cutter so much longer than the diameter I feel like sword fighting. "ENGARDE!" I have a 3 flute, 2-1/4" LOC, center cutting on order. That was like pulling teeth, and it's only $40.

 

Anyhow, Beej, sorry man... can't get any more tools in there. The drill is there mostly because this rougher isn't center cutting.. plus I'd like to give the chips a way to get out of the way. Not your fault.. I should have given more information ... like I am now.

 

Finally the speeds and feeds, "S2037 F24.444" are from Mastercam X from material. What the Fu-hell? I agree, too conservative. I tried from default and from tool but from material was the fastest of the three. Of course, I could be doing something horribly wrong there and not even know it. Cranked it up to S12000 F65 and got a "holy [crap]" from two guys with over 20 years experience each. Made me proud, thanks guys. Where are you getting that SFM? I've searched both the 26th and 27th edition of the Machinery's Handbook and it gets pretty vague when dealing with a butter soft material. Like butter, you can chop at it really easy with a chainsaw, but sculpting it ... slow down. I even broke a 1/2-14 NPTF in this junk.

 

 

Sigh.. I need to get back to harder material that does what I tell it to. Again ... thanks guys.

[Guest]

If you've got Machinery's 26th Edition on page 1007 Table 8

 

 

It's a good starting point 2820 SFM

 

If you have a rigid setup and you are not getting at least 2000SFM you are not working either the tool OR the machine

 

When in a hole like you described, I'll ease of the feed rate a bit to get better chip evacuation but if I have an open area to cut I'm pushing 185 - 225 IPM

 

BTW, 4 flutes an aluminum s*ck

 

I always prefer 3 flutes and I'll take a 2 flute before a 4 flute/

[LT_mechead]

It sounds like you've got the problem solved to your satisfaction. However, don't think that you need a center cutting endmill to do a helix bore. I've done helical pocket entry with facemills. You just have to be careful in setting the helix angle and radius so that: 1, The teeth on the back side of the cutter are not presented more material than the width of their cutting edge. And 2, The endmill traverses a distance greater than the uncut diameter.

 

That being said, I recommend you stick with the drill until you get the new cutter. The cutter you are using have will have problems clearing the chips in Al, and it will howl like a b*#$@ on a helix bore.

 

Lee

[Sambo]

That's awesome. lol one more thing I left out ... it's not carbide ... and yes it's screaming, it was screaming from the get go with the slower speeds and feeds so I didn't think too much of it. That new endmill should come in on Monday.

 

John, I've been over that book a thousand times ... how could I miss that?

[Guest]

quote:

---

John, I've been over that book a thousand times ... how could I miss that?

---

You need to take a couple of reading lessons from Hardmill meh thinks and learn to only look at the pictures

 

 

quote:

---

it's not carbide

---

There's something else to cut aluminum with besides carbide?

 

Whoda thunk it?

 

[Ballnose Bill]

Sambo, tooling is everything.I use HSS 1% of the time.Worth every penny. For aluminum, Mini-cut from international(competively priced too) is pretty slick, I don't have the spindle to get 2500 SFM but can cut full dia depth spinning 6700 at 85 IPM no problem. Although not the best application for helical boring at full dia.Can you get 1 15/16 insert drill. Even drilling with carbide followed by a insert counterbore(Can hold .002 tolerance) would fly compared to HSS helical bore.

[daryl_y]

Our shop cuts aluminium with Clevland Twist Drills series 538 and 539 endmills. for roughing with a DOC at about 50% of the cutter dia I would run a sfm of 1000 and chip load of about .004 per tooth using this tool in an application that use described a rpm of 5600 and feed of 67 ipm would be no problem at all. Your feed could likley be mush faster than that since you are ramping and you doc would be likley be mush less 50% of your cutter dia.

 

I agree with the others I would probably loose the drill and ramp the hole out.

[Sambo]

Just thought I give everybody a heads up on where things are now, and a thank you also. I got the three flute rougher on Monday, and wow what a difference. The through hole is gone. Hey it only took two weeks from when I asked for the rougher, but thats business as usual around here, didn't even have material until the whole order was due. I'm amazed we don't have tons of these tools around here with so much aluminum and brass work we do. And I'm more amazed we're still in business.

 

Before I got my hands on this part, it was being run in two operations and making 4 parts a day. I've got it all in one operation/setup and I'm making 7 a day. I want to hit 8 but with the chip bin on this thing the size of Keebler's bath tub, I have to clean it out twice a part. I have a good arguement for a chip-conveyor here. Quoted at $5600 should be here in 2 weeks (haha I'll believe it when I see it). But still have over 100 parts to go, so that chip conveyor will get a good break in.

[Guest]

quote:

---

but with the chip bin on this thing the size of Keebler's bath tub

---

http://plugin.smileycentral.com/http%253A%252F%252Fwww.smileycentral.com%252F%253Fpartner%253DZSzeb008%255FZNfox000%2526i%253D36%252F36%255F11%255F6%2526feat%253Dprof/page.html' target="_blank">

[Thee Rickster ™]

lol!

[Hardmill]

quote:

---

You need to take a couple of reading lessons from Hardmill meh thinks and learn to only look at the pictures

---

Hey I resemble that

 

 

PEACE