Ramp Angles for Aluminium / Aluminum

[m_morgan]

For all the guys machining Aluminum or Aluminium (depending on whether you think it's a gray color or a grey colour), what ramp angle do you use for entering pockets and why?

[Flycut]

It really depends on the cutter you are using.

I usually plunge with solid carbide endmills.

[crazy^millman]

Depends on the cutter all cutters have a recommend ramp angle in the book. Some allow up to 30 deg some only allow 3 deg so it depends on that aspect of it. I do a standard amount 99% of the time that way I know exactly what I am getting when doing parts when using the angle in ramp if you have a long contour and it is set at 3 deg you might end up with 1" depth of cut on a long chains where as with controlling it using a certain depth you know you get what you want and do not end up with unpredictable depths when doing different chains and shapes in the same part which require you to play with the angle which cost time when programming.

 

HTH

[ReDEyZZ]

if you use a 2 flute carbide "bright finish" is a good way to go, you can ramp at any angle or plunge straight down. if you are using an indexable carbide endmill with special aluminum inserts, you have to check with the specs for maximum ramp angle. as to the grey color??? what kind is it? cast?? billet??

[Rick Henrickson 65]

+1 crazy 3 deg for endmills, now inserted endmills you need to check your catalog for specs.

[m_morgan]

I'm working a lot with forged billets at the moment, and they can bow and twist quite considerably depending on the machining technique.

 

From speaking to a very wise learned Engineer in a different company, he reckons that by ramping at a shallow angle, you're grinding or smearing the material off, and generating a lot of heat within the stock. By ramping or plunging, you heat the ships, and keep the billet from warping.

 

Is it that simple?

[gms1]

Im using mitsubishi's bxd line of indexable cutters for aluminum and I usually ramp @ 18 degrees. The book says I can do 20 degrees but I usually cut it a little short just to stay in range and be a tad more safe.

[Chris Rizzo]

quote:

---

From speaking to a very wise learned Engineer in a different company, he reckons that by ramping at a shallow angle, you're grinding or smearing the material off, and generating a lot of heat within the stock

---

typical engineering logic

 

Aluminum cutting generates chips, the only time your smearing the material is if your cutter is galled up. As for heat, are you machining dry?

[mold100]

Coolant a must for me, I am a plunger, 1/2 dia Garr 3 flute aluminum cutter, I go .200 deep 8400 rpms, plunge at 20ipm, and cut 210 ipm. certain things I ramp usually 3 to 7 degrees depending on how open and cutter bottom geo. I also use data flutes regulary and plunge, no probs with heat generally.

[crazy^millman]

Ok then how did he recommend you get into a pocket when milling if you are not going to plunge or ramp? If you are ramping at a shallow angle would it not be the same as taking a small finish cut in the bottom of a pocket. The only time this would be an issue is by some chance you are not using a bottom cutting endmill. If the endmill or tool is designed to ramp then the bottom edge of the tool is designed to cut and if you were taking a shallow cut and feeding at the correct feed rate using the correct ramp angle or less for the tool then all the heat and stress will og in the chip. We are doing some parts right now heat treated to 55 rc and I got a tool for them to run dry. They did not run it dry and the 1st 2 parts came off warped. They then ran the rest of the part dry and the parts are within .001 flat. The tool has the same principle as an Alum tool where the heat and stress come out in the chip and not into the material if run the right way.

[m_morgan]

Thanks for all the replies guys!

 

I've been following the manufacturers reccommended speeds and feeds, and the Makino Mag3s have plenty of coolant flow to keep the heat down at the cutting edge.

 

Basically, the full story is that I'm testing a 25mm 3Flute (1/2"(ish))cutter, which is cutting at 33000rpm F18000m/min (700imp). At that speed, I don't fancy ramping very hard, but I am also aware that I can produce quite a bit of heat if the cutter is not cutting effectively.

 

The general statement by this other guy seemed a bit off the top of his head, hence all the questions in this thread.

 

Just another question - Mold100, what are data flutes?

 

Thanks for the help guys!

[Guest]

quote:

---

what are data flutes?

---

Data Flutes are a Brand name cutter

 

Linky