304 SS @ 24 IPM

[thum31]

I found an article on high speed machining yesterday. I changed one of my programs using the formulas recommended and WOW. Cut cycle time from 38 minutes to 8 1/2.
Using a 4 fl 1/4 carbide tiAln I set it up to cut a depth of .625 at 1750rpm at 18.375 ipm. once the part started I had a little squeal so I bumped up the feed to 24ipm.
I will add a link to the article if I can find it. It is really worth the read.

http://www.cuttingtoolengineering.co...12-Milling.pdf

[thackman]

Are your running dry, flood, or mist? What was the width of the cut: 100% (slotting) or 50%, 30% ,25%, etc (profiling)?

[thum31]

It was an internal pocket spiraling outward from the center, and an external contour. Food, at .012 woc. I followed the calculations in the article pretty close then made a few adjustments. The article said to take the required DOC and divide by 2.5 to get the end mill size. .625/2.5=.25. then take your normal clpt and multiply by 3.5 and calc the speed and feed with that number. I use .00075 normally times 3.5=.02625*4*1750=18.375

I picked 1750 for the rpm thinking that pully would provide more torque.

This is supposed to keep the chip size the same (.00075) but now it is .625 tall. the writer was looking at using the full cutting edge of the given tool.

[BobWarfield]

Great article, thanks for the link.

Best,

BW

[zephyr9900]

It was an internal pocket spiraling outward from the center,

How did you start the pocket, thum31? Did you drill or plunge a pilot hole or just ramp the cutter down? If the latter, it seems like the cutter would have a big chip load for a while because you're effectively slotting at the start. Was it regular spiral pocketing or does your CAM do the trochoidal thing (which I'd love to try someday but SheetCam doesn't do that...)?

Thanks,

Randy

[keithorr]

Thank you for the link. I'm looking forward to trying the numbers on the next appropriate job.

The last lines of the article read:

"Steele said he is somewhat reluctant to use the term
“breakthrough,” but feels “we are pretty close to redefining
the way people ought to be machining. In our battle with
offshore competition, we have to be smarter. Automation
and techniques like this are going to help us win.” "

Win what? What's to prevent an offshore vendor from buying the tooling, software, machines and doing the same? You think Seco or Iscar will limit who buys their tooling?

[thum31]

Randy,
I had a .375 pilot. I fdrilled the part before parting off the material. Regular spiral starting in the center. I had another fo at it today. I ran it with a .122 woc at .600 depth. 32ipm Things were going great till I lost the battle with chip evac. Once that happened the spindle started to slow so I had to abort. If the chip could fall out the bottom I think that it would have been fine.
I am thinking about the new spindle in the future.

[hawkburger]

I use the dia. of cutter to set the max amounts for toolpath depth and width.
Usually going for 100% depth x 50% width.; preferably
but for slots it would be vice versa. 50% for depth and 100% for width O.K.?
depth. = 50%of cutter dia. for depth of cut. x 100% for width of cut.
(and vice-versa.)
So for contouring it's 100% of cutter for "depth" x 50%of cutter for "width" of cut.(Preferred)
Slotting : Start a Ramp angle 3deg.(5deg. if you want to max output) "zig-zag" and "criss-cross" down to 1/8 deep. Feed rate 50% of linear feed(5.0 I.P.M.).
'Zig Zag' and 'criss cross' gets to depth with less downward (Plunging) force. and cuts without rubbing the center of tool as much as constant circular ramping.
"As long as the ramp strokes are 200% larger than the tool dia." (1 inch)
This allows for Chip evacuation!!!!!!!
This saves the work hardening of Matl. for further machining ease.
When the ramping is at 50% of tool dia. deep. then linear feed 10.0 I.P.M.
My speed for 302 stainless with tialin Carbide = 165 SFM 1/4 mill tialin
2521 R.P.M.
.004 feed per rev. = 10 inches per minute.
( Small slots ramp-cut with 3-flute flat endmill 50 % Feedrate)
That cuts a .125deep slot 1/4 inch wide 10 inches long in one minute.
If you want high speed machining try using Rounded ball endmills not flat ones for rough milling slots.
My tools cost money and I have plenty of time, just not alot of money.

[sharpshooter90]

"Steele said he is somewhat reluctant to use the term
“breakthrough,” but feels “we are pretty close to redefining
the way people ought to be machining. In our battle with
offshore competition, we have to be smarter. Automation
and techniques like this are going to help us win.” "

Win what? What's to prevent an offshore vendor from buying the tooling, software, machines and doing the same? You think Seco or Iscar will limit who buys their tooling?

In our present economic situation, i think you will find that there is a plentiful supply of skilled operators willing to work at low wages available here in USA. For highly technical work, often 90% of the expense is in the equipment, so cheap foreign labor is not that big of an advantage. Adding the costs of importing specialized materials and then re-exporting them, offshore companies would not have significant advantage.

[300sniper]

I found an article on high speed machining yesterday. I changed one of my programs using the formulas recommended and WOW. Cut cycle time from 38 minutes to 8 1/2.
Using a 4 fl 1/4 carbide tiAln I set it up to cut a depth of .625 at 1750rpm at 18.375 ipm. once the part started I had a little squeal so I bumped up the feed to 24ipm.
I will add a link to the article if I can find it. It is really worth the read.

http://www.cuttingtoolengineering.co...12-Milling.pdf

i read over that article again and gave this technique a try today.

the material was 1018 cold roll steel. i used a 1/2" tialn four flute carbide endmill at 2254 rpm. a .010" radial doc, 1.000" axial doc and 60 ipm. i ran it dry and it performed extremely well. in the about 40 minutes of machine time, i created quite the pile of chips.

i had access to 3 sides of the part so i cut a slot on the side that had no access. once that was opened up, i climb milled around the profile the full depth with .010" step over. the long chips were flying and creating a few large piles of chips. i was nervous at first but soon found myself impressed watching a 1/2" cutter at 60 ipm in steel.

i didn't shove these chips into these piles, that is just where they landed during the machining.

[BobWarfield]

Radial chip thinning is a beautiful thing:



In fact, you have to crank the feeds way up just to get the same effective chip load as with a more normal depth of cut. Failure to do so can leave you cutting a chipload that is less than the radius of your cutter's edge. Suddenly you're rubbing instead of cutting and your tool life will go down in a hurry.

Figuring all of this out automatically is why I originally created my G-Wizard calculator. In fact, this particular cut would need to run at 86 IPM (if you had that much feed) to restore a normal chip load of 0.0014".

Bumping the SFM can be a little dicier unless you really know exactly what your toolpath is doing by way of cutter engagement. If you get it right, you are flying along the way CAM products like Surfcam do. If you get it wrong, you're burning tools. Takes a lot of spindle rpm to get there though.

Meanwhile, it sure is cool to pile up those chips that fast!

Cheers,

BW

[keen]

Hi - At those speeds are you not getting stepper coupling 'creep' or even steps loss due to the rapid reversals? I find I start to lose position if the speeds are too high..