cutting aluminum

[Travis2282]

I have recently been cutting aluminum and have had problems with my thin pockets cutting shallow in the center and even some cutting all the way through. i should have .01-.015 thickness but not sure if the material is sucking up as i cut or what.

[Guest CNC Apps Guy 1]

Without seeing the parts, that's what I would infer.

 

Try using reverse flute endmills (spiral down as opposed to spiral up). Then will force the cutting pressure down. Or, don't cut the pocket in steps. Spiral down to finish depth in the center and spiral your way out taking less radial cut than usual. I've dont that n the past.

 

HTH

 

Welcome to the forum

[TheePres]

At .010-.015 its almost necessity to use a vacumn.

[crazy^millman]

Like James without seeing the part same thing left hand spiral cutting end mills. I worked at a place where we did .003 thickness floor in plastic and used them and they worked great and held thickness all day log.

 

HTH

[Camdude®]

+1 on reverse helix, We used reverse helix on thin floors with plastic and alum it it worked great. With plastic we had to watch the chip flushing.

[CNC PRO]

Not to hijack this thread...too much, I am a wood guy but have machined aluminum on the routers a few times and may have to again sometime, could I ask what my RPM's, IPM's should be at?

 

I was using a down spiral solid carbide with a 800-1000RPM @ 50ipm...which sounded rough and left light chatter marks on the floor of the part. Are my rpms too low, ipm too high,wrong tool? sounds like I got the spiral right at least.

I realize that different grades would mean different settings(or I would assume), I just need a general idea....thanks

[Namliek_J@TheeCircle™]

quote:

---

I was using a down spiral solid carbide with a 800-1000RPM @ 50ipm...which sounded rough and left light chatter marks on the floor of the part. Are my rpms too low, ipm too high,wrong tool? sounds like I got the spiral right at least.

---

What size and type of tool? How many flutes? How thick was the aluminum?

 

If you are running 800 RPMs @ 50 IPM, that is a chip load of .0625 inches per rev. That is pretty high.

 

Need a little more info to give you a better answer.

[CNC PRO]

The tool was a .4375"dia. 1" cut hieght, Solid Carbide Down spiral 2flute.

The aluminun was 1/4" thick.

 

 

Thank you for your reply

[Hidalgo]

Clean part with acetone and use

3M double sided tape to tape a block

underneath to support the floor.

[CNC PRO]

quote:

---

Clean part with acetone and use

3M double sided tape to tape a block

underneath to support the floor.

---

Thanks, but I don't believe hold down was the issue though...as I had this part clamped and vacumed down, seemed fairly solid.

[MLS]

A radius on the EM will give you some downforce as well, but not as much as a reverse helix.

 

Another thing you can do is leave more material on the floor during rough, start in the middle, and melt out( semi-finish/ finish/step out radially/semi-finish/finish/step out radial/etc.) similar to the way you would melt down a flange.

 

CNCPRO

Most aluminum can be cut without a limit to RPM. We run a .500 carbide at 30,000 RPM and I know there are machine that go even faster. It is extremely forgiving if its held in a rigid state.

[Namliek_J@TheeCircle™]

CNC PRO,

 

Depending on your machine, you can run that tool at very high speeds. I would start around 1000 SFM, and about .008 IPR and test it out. That gives you 7640 RPM @ 61 IPM. You can them up the speed and feed if you machine allows.

[CNC PRO]

Thank you J.Keilman and MLS for your help.

[robh]

If your part was very wide even tho your using a vacuum the clamp you are also using could bow the part up in the center.You've probably thought of that I'm sure.

Regards

robh

[mike_f]

I'm curious, I've used "left hand helix, right hand cutting " end mills for thin wall sections ( with fixturing to support the opposite side of the wall ) but because of the negative angle on the end of the end mill I've never had any success milling floors with them. insted of "shearing" material up and away from the cutter, they "plow" the material down and into the face you are machining. usually resulting in galling and poor surface finishes....so, my question to those of you who have had success milling floors with these tools is how have you applied them ?...I know the question is vague, sorry. Thanks in advance for any advice.

mike