Aluminum cutting speeds with an X3

[carvemylog]

I have a CNC router which I'm using to cut hardwood and some aluminum. It cuts the aluminum fine with a 1/4" carbide router bit, but is slow. The fastest I seem to be able to cut is 15ipm with a 0.025" depth of cut.

I've never run a mill befor, so sorry for the newbie question, but should I upgrade to an X3 in the future to cut the aluminum parts I need, what kinds of speed and depth of cut I could get out of one with a 1/4" end mill.

Thanks

[hoss2006]

Have you tried using an endmill instead of a router bit?
You can get them in 1/4 inch shanks.
Sherline sells some for one.
You probably won't have the rigidty to go deeper but you should be able to feed faster.
An X3 will get you much higher depths of cut.
Hoss

[David Da Costa]

I am using 3 flute accupro aluminum or 2 flute Fullerton Aluma end mills on my smaller KX1 and cut at 17ipm with 0.3 ipm at 7,000 RPM with drop coolant (trico md-1200) with great finish on the cut surfaces so you should be able to exceed that.

I agree with Hoss, you need to use an end mill not a router bit.

David

[BobWarfield]

I ran these numbers through my G-Wizard feeds and speeds calculator and came up with the following:

For a 1/4" carbide 2 flute in aluminum, assuming a max spindle rpm of 4000 (not sure what it is on those siegs), a full width slot would be cut at 16 IPM. However, if you drop back to a light cut (probably better for a light mill anyway) and use High Speed Machining techniques (radial chip thinning is the buzzword), you can cut a 0.010" depth of cut at 80 IPM.

There are parts in between, of course, but anytime you cut less than 1/2 the diameter of the cutter, you can take advantage of chip thinning and just increase the feedrate. For example, a 40 thou depth of cut can run 40 IPM.

The trick is knowing how much. Those calculations are what G-Wizard does.

If you want to try it, go here:

http://www.cnccookbook.com/CCGWizard.html

Chip thinning is cool stuff. I was cutting some steel at 35 IPM

the other day and it was smooth as silk on my IH mill. Very quiet, nothing got too hot, and life was good. I would not have suspected I could go that fast as without the chip thinning calculation, the suggested speed would be single digit IPM.

Cheers,

BW

[HimyKabibble]

Originally Posted by BobWarfield I ran these numbers through my G-Wizard feeds and speeds calculator and came up with the following: For a 1/4" carbide 2 flute in aluminum, assuming a max spindle rpm of 4000 (not sure what it is on those siegs), a full width slot would be cut at 16 IPM. However, if you drop back to a light cut (probably better for a light mill anyway) and use High Speed Machining techniques (radial chip thinning is the buzzword), you can cut a 0.010" depth of cut at 80 IPM. There are parts in between, of course, but anytime you cut less than 1/2 the diameter of the cutter, you can take advantage of chip thinning and just increase the feedrate. For example, a 40 thou depth of cut can run 40 IPM. The trick is knowing how much. Those calculations are what G-Wizard does. If you want to try it, go here: http://www.cnccookbook.com/CCGWizard.html Chip thinning is cool stuff. I was cutting some steel at 35 IPM the other day and it was smooth as silk on my IH mill. Very quiet, nothing got too hot, and life was good. I would not have suspected I could go that fast as without the chip thinning calculation, the suggested speed would be single digit IPM. Cheers, BW

Bob,

Everything I've read re: HSM indicates the HSM rules only come into effect at SFPMs on the order of 10X or more the conventional machining values. That, of course, means spindle speeds FAR in excess of what our machines are capable of. My understanding is you *can* push the tools as you suggest, but tool life will suffer greatly. What has your experience been? Using (aggressive) conventional techniques, my tools seem to last almost forever - I've been using most of the same endmills for most of the last year. Mine now tend to be retired mostly due to abuse/stupidity (like doing a rapid into a clamp), not being worn out.

Regards,
Ray L.

[BobWarfield]

Ray, SFM burns up cutters. Chip thinning is not about increasing the SFM at all. In fact, as you know, my mill has a very slow spindle on it, so it's hard for me to exceed (or even get to) recommended SFM for most operations.

Compensation for chip thinning, lead angle, and ballnose cutters (all things G-Wizard does) are all geometric effects.

Chip thinning is a function of the idea then when your spinning cutter is in a depth of cut that is less than half the cutter diameter, it actually doesn't cut as thick a chip at a given feedrate as for depth of cut greater than or equal to half diameter. In fact, what the calculation does, is simply to figure out how fast you have to feed just to get the same chip loading as would naturally occur were you cutting deeper.

Hence, it works great with no impact on the tool life that is noticeable. As I mentioned on my steel cutting example, the machine ran very smooth and nothing got too hot at all. It was remarkably quiet. Those are all good signs, but don't take my word for it. Go out and search for "chip thinning" on Google.

I'm surprised more people don't follow the practice. Heck, even my CAM program doesn't seem to bother, and it sure makes a difference.

BTW, a combination of chip thinning and cutter engagement compensation are what pass for a lot of the HSM CAM toolpaths, like trochoidal cuts. When you can generate toolpaths that automatically take all that into account, your machine can really fly!

Cheers,

BW

[HimyKabibble]

Originally Posted by BobWarfield Ray, SFM burns up cutters. Chip thinning is not about increasing the SFM at all. In fact, as you know, my mill has a very slow spindle on it, so it's hard for me to exceed (or even get to) recommended SFM for most operations. Compensation for chip thinning, lead angle, and ballnose cutters (all things G-Wizard does) are all geometric effects. Chip thinning is a function of the idea then when your spinning cutter is in a depth of cut that is less than half the cutter diameter, it actually doesn't cut as thick a chip at a given feedrate as for depth of cut greater than or equal to half diameter. In fact, what the calculation does, is simply to figure out how fast you have to feed just to get the same chip loading as would naturally occur were you cutting deeper. Hence, it works great with no impact on the tool life that is noticeable. As I mentioned on my steel cutting example, the machine ran very smooth and nothing got too hot at all. It was remarkably quiet. Those are all good signs, but don't take my word for it. Go out and search for "chip thinning" on Google. I'm surprised more people don't follow the practice. Heck, even my CAM program doesn't seem to bother, and it sure makes a difference. BTW, a combination of chip thinning and cutter engagement compensation are what pass for a lot of the HSM CAM toolpaths, like trochoidal cuts. When you can generate toolpaths that automatically take all that into account, your machine can really fly! Cheers, BW

Bob,

So you're applying chip thinning to normal square-tipped endmills? What I've read on chip-thinning applies to ball-nosed mills, feed mills, and other round-edged tools. I've never seen it applied to normal square endmills, as the chip thinning effect is a result of the curved cutting surface. If it helps get things done faster, without seriously compromising tools life, I'm all for it, I've just never seen it applied to normal endmills.

Regards,
Ray L.

[BobWarfield]

Originally Posted by HimyKabibble Bob, So you're applying chip thinning to normal square-tipped endmills? What I've read on chip-thinning applies to ball-nosed mills, feed mills, and other round-edged tools. I've never seen it applied to normal square endmills, as the chip thinning effect is a result of the curved cutting surface. If it helps get things done faster, without seriously compromising tools life, I'm all for it, I've just never seen it applied to normal endmills. Regards, Ray L.

Chip thinning works in either the axial or the radial plane. The chip thinning you refer to for button cutters and the like is axial and is a function of the geometry of the cutter nose. I'm referring to radial chip thinning.

Take a look at the G-Wizard page near the bottom for an explanation of the geometry for radial chip thinning. It isn't dependent on the cutter shape so much because viewed from the axis of the spindle, the cutter is round by definition as it is spinning. Not hard to understand, but very effective in practice.

Cheers,

BW

[HimyKabibble]

Originally Posted by BobWarfield Chip thinning works in either the axial or the radial plane. The chip thinning you refer to for button cutters and the like is axial and is a function of the geometry of the cutter nose. I'm referring to radial chip thinning. Take a look at the G-Wizard page near the bottom for an explanation of the geometry for radial chip thinning. It isn't dependent on the cutter shape so much because viewed from the axis of the spindle, the cutter is round by definition as it is spinning. Not hard to understand, but very effective in practice. Cheers, BW

Bob,

Ah, that makes sense. I guess I've unknowingly applied the principle, but more experimentally. My tool parameter generator does provide essentially that compensation, but derived more by trial-and-error, rather than calculation. Time to do some more programming!

Regards,
Ray L.

[carvemylog]

Thanks for the replies. Would an end mill work OK at the higher rpms a router turns? I cut a 3/4" 7075 plate of aluminum yesterday with a router bit and it did a good job other then taking forever at 0.25 doc. I only sprayed a mist of water on the bit for coolant. Do you think I could increase the doc using an end mill and only a water as coolant?

Thanks

[SlowRiderr]

Originally Posted by carvemylog Thanks for the replies. Would an end mill work OK at the higher rpms a router turns? I cut a 3/4" 7075 plate of aluminum yesterday with a router bit and it did a good job other then taking forever at 0.25 doc. I only sprayed a mist of water on the bit for coolant. Do you think I could increase the doc using an end mill and only a water as coolant? Thanks

Never use water alone without coolant, even it if is aluminum. What about your tooling and machine?

Also calculate your feeds based on your RPM. And you mean .025 instead of .25 DOC?

[HimyKabibble]

Originally Posted by carvemylog Thanks for the replies. Would an end mill work OK at the higher rpms a router turns? I cut a 3/4" 7075 plate of aluminum yesterday with a router bit and it did a good job other then taking forever at 0.25 doc. I only sprayed a mist of water on the bit for coolant. Do you think I could increase the doc using an end mill and only a water as coolant? Thanks

At 25K RPM, you should be able to do true high-speed machining, which means shallow cuts, very fast feed rates, and no coolant. But a router bit will be less than ideal, as the rake will be wrong for aluminum, and they're also not nearly as sharp as an endmill.

I've been tempted to make a mount to put a router head on my mill to try some HSM, before sinking the money into a real high speed spindle....

Regards,
Ray L.