trouble with the slot

[Uman]

What is the best practice for slotting aluminum? I need to mill an endless supply of slotted parts and do it efficiently and fast. I have an 1100 with dual fogbusters and need to cut 1/4" thru slots .375" deep.
My past experience has been painful and would like to increase my parts per em. I am using a 2flt carbide em with short stickout very conservatively, but maybe to much and that is the problem.
Discussion on cutter type, DOC and F&S would be most helpful.
-uman

Similar Threads:

• Trouble cutting circles. Trouble with y-axis
• How to slot a rectangular slot with convex bottom ?
• one slot is coded other slot is not there
• cutting a slot with a t-slot cutter
• Coated Carbide 4Flute Endmill, 3Flute Slot Drill, or 2Flute Slot Drill?

[RussMachine]

How tight is the width tolerance on that slot? .250 +/- ??

Definitely go with a 2-Flute Endmill.
I would fly through it with two passes, to put less stress on the endmill.
.187 deep X positive move, first pass.. then .375 deep coming back through the slot, X negative move.
Two quick passes, and DONE!
5000 RPM at 40 Inches Per Minute, with full coolant (or mister blast).

[MichaelHenry]

Why is a 2-flute end mill better than a 3-flute? I'm almost positive I've seen 3-flute recommended as the way to go for slotting.

[cobrakai]

I would use a 3 flute 1/4", 5100rpm, 28IPM, .1875 depth per pass. That's just extrapolating parameters I've used before that worked well. If tolerance and surface finish is important, you'll probably have to use a 3/16" and do a 2D contour with a finish pass. Getting the chips out is KEY. Direct the blast so they push the chips backwards away from the cutter.

[Jim Dawson]

A 3 flute would be fine, it would allow a bit higher feed rate and the web is a bit stronger than the 2 flute. Just get one with a geometry designed for aluminum cutting. You might get better accuracy using a 6mm (0.239) endmill rather than a 0.250 that way you are only cutting on one side of the finished slot at a time. Maybe keep the chip load around 0.002 or so. Unless you drill a pilot hole you will need to ramp into the cut, maybe 2° or so. I think you can do it in 2 passes of 0.188 depending on the accuracy and finish required.

[Steve Seebold]

I use a Fogbuster as well, but a Fogbuster does not work for slotting. You need to be using flood coolant and a good 3 flute end mill.

I would like use a 3/16 3 flute end mill and go thru your part in 4 passes to get to desired depth then finish the side walls.

As much as I like the Fogbuster, it's not the coolant delivery system. It just doesn't deliver the right amount of coolant for slotting.

[davebaldwin]

No expert myself but have a look at this video by NYC CNC on slotting.



Dave.

[Uman]

RussMachine
How tight is the width tolerance on that slot? .250 +/- ??

The slot width tolerance is very loose and is just for aesthetics, but is limited to maybe .300" wide.

Steve Seebold
I use a Fogbuster as well, but a Fogbuster does not work for slotting. You need to be using flood coolant and a good 3 flute end mill

Yea Steve, I believe the problem is the Fogbuster in this application. It just does not provide adequate chip evacuation in the depth of the slot.

The 2flt vs 3flt em disagreement may be due to the coolant technique. Could it be flood users prefer 3flt for rigidity and speed and foggers prefer 2flt to leverage chip evacuation?

davebaldwin
No expert myself but have a look at this video by NYC CNC on slotting.

Adaptive slotting may be the solution for Fogbusters. Would a 3/16" em work to adaptive cut a .250-.300" slot?

[tbev]

I've pushed a lot of different 3/16 em's recently and the Destiny Viper is the best finish and removes the most material the fastest. I don't think you can find it with that short of a LOC which is going to be key for you in this cut. You want the minimum required stickout and LOC I would also recommend a 30 to 37° helix, rather than a 45°or higher.

Sent from my SM-G900V using Tapatalk

[Steve Seebold]

No expert myself but have a look at this video by NYC CNC on slotting.



Dave.

I've watched some videos from NYC CNC and I noticed he gets a lot of chip welding, especially when he cuts aluminum. I think his biggest problem is he's just cutting in the wrong direction.

Well, I just watched his video and I take back any negative remarks I posted above.

[tbev]

Did you try an adaptive pass?

Sent from my SM-G900V using Tapatalk

[Uman]

tbev
Did you try an adaptive pass?

This will be my next attempt if slot fogging is possible, but I will need to open the slot to .300" wide and get a good quality 3/16 em (2-flt 3-flt I will try them both)

Steve Seebold
I use a Fogbuster as well, but a Fogbuster does not work for slotting. You need to be using flood coolant and a good 3 flute end mill.

Steve, you flood and fog, are you saying slot flooding is a must and slot fogging is not practical for production work?

[wildwhl]

Just a suggestion - but I've had great luck "slotting" by using a slightly smaller end mill than the slot, and running the contour in a (ramp) pattern (or plunge, cut, plunge, cut). For example, if your slot has to be .250", use .1875" end mill and zip around and down in maybe 3-4 runs, with a finish pass at the end. Note: I run flood coolant all the time, so maybe this is why this works so well for me

If you can be .260" or larger, use the 1/4" end mill and run faster/harder.

Just an idea.

WW

[tbev]

I also use that contour ramping method, works great! Destiny Viper 3fl. I'd the best I've found, I broke the of them today, but they are still the best I've found..

Sent from my SM-G900V using Tapatalk

[AUSTINMACHINING]

Getting the chips out as others have said is the key to making it work. If you don't have blast flood available, I would try ramping fast in a zig zag profile at a shallow angle to keep the chips small/easier to get out. High pressure air blast would help a lot. I just did a 4" x .6" x 2.1" deep slot with a 1/2 " end mill. I did a contour ramp at 3 degrees and 50 Ipm and,left .005 for a finish pass. Got a little crunchy, but worked out fine. This was a blind slot, not through, but using flood cooling. If it was a through slot, I would drill out the corners all the way through first before slotting.

[Steve Seebold]

This will be my next attempt if slot fogging is possible, but I will need to open the slot to .300" wide and get a good quality 3/16 em (2-flt 3-flt I will try them both)



Steve, you flood and fog, are you saying slot flooding is a must and slot fogging is not practical for production work?

When I try to slot using the Fogbuster, I'll wend up with 2 pieces of carbide. One is all shank and the other is all flutes. But I have never tried th slot the way John did.

[GJeff]

I'm currently troubleshooting adaptive slotting recipes in this thread http://www.cnczone.com/forums/autode...2-tormach.html
And I'm running into severe limitations due to acceleration at high IPM. If I can get those solved, I could have some really nice slotting times w/ mist coolant using the full length of the flutes.

[IMT]

I have found that HSM tool paths don't work well for small slots in aluminum on the 1100. Since the tool path radius is so small, the feedrate has to be adjusted down so the chipload at the OD of the tool is accurate, vs the feed at the center of the tool. The acceleration of the machine must also be considered. After all this is accounted for I found that it takes 2-3X longer than just full slotting at a reduced DOC. The tool will wear out faster since only the bottom .1 or so is being used, but in aluminum it still lasts long enough.
Slotting in stainless or alloy steel is a different story since the tool life will be much less and cost of extra endmills may outweigh the time savings.

[popspipes]

What is the best practice for slotting aluminum? I need to mill an endless supply of slotted parts and do it efficiently and fast. I have an 1100 with dual fogbusters and need to cut 1/4" thru slots .375" deep.
My past experience has been painful and would like to increase my parts per em. I am using a 2flt carbide em with short stickout very conservatively, but maybe to much and that is the problem.
Discussion on cutter type, DOC and F&S would be most helpful.
-uman

What type is the aluminum?? I didnt see it mentioned , some of it is very gummy and doesnt machine well at all.

I SLOT AT 45 ipm .250 3 flute carbide, .130 DOC full width, approximately 2 feet per part 2 passes, havent broken a cutter yet,on one of the parts I make.
I do use flood diesel/hydraulic oil mix.

Right or wrong its just the way I do it..........

edit: 6061 T6 is what I am using, cheapest of the good machining grades.

[Jim Dawson]

There is a definite problem removing chips from a narrow slot, but it is doable. A high pressure flood system works well, but a low pressure system is marginal at best. If you don't have high pressure capability or your machine is not equipped for handling a flood coolant system then a mister system is the only real choice. The problem with the mister is that most of the commercial systems use a syphon to induct the coolant into the air stream. This requires a balance between the air flow and the fluid stream with very limited adjustment range.

I solved the problem by making my own ''fogbuster'' system with a pressurized fluid delivery system with independently adjustable air and fluid flow. I can adjust the airflow up to whatever air comes out of the nozzle at shop air pressure (140 PSI), and it will still deliver a set amount of fluid per minute in the range of 0 to flood. I built a peristaltic pump for the fluid delivery and use a stepper motor to drive it. You can also buy stepper powered peristaltic pumps on ebay for cheap. I have it under computer control, but it could be a separate controller. You can set the airflow hard enough to blast the chips out of the slot, and still deliver the proper amount (minimum required amount) of coolant to the tool bit. For aluminum, kerosene is my favorite cutting fluid.

Here it is at about 10% fluid flow



and at about 40% fluid flow. Note the ''no fog'' small droplets