What's new
What's new

Questions on using a gang of slitting saws?

mastuart

Aluminum
Joined
Feb 25, 2013
Location
Mendota Il USA
Hi guys. I have a little project using slitting saws. Saws are 1.750 dia .040 thick with a .040 thick spacer between them. They have 90 teeth each. The material to get slotted is 6061. The questions are. Is it better to clime mill or conventional mill with them? What way will give the best results regarding a burr free surface. How fast should I turn them? What feed rate? What about lube? Also the slots are .050 deep. should they be cut in one pass or more than one? I don't have flood coolant. I have about 70 more to do and so far I am not happy with the results.

104_0737.jpg
 
You want courser teeth with Al, especially the softer alloys like 6061. Your setup needs flood or mist cooling, somehow you've got to kluge something together to allow it. Even an aquarium pump and basin is better than nothing.

Climb mill, multiple coolant outlets to ensure the part doesn't mask the flow, high spindle speed if those are carbide saws, and ensure they're running true - wobble or poor TIR hurt with slitting saws.

Burr free is likely not happening with soft Al, not without very sharp cutters and coolant to keep the forces low. Or do a peripheral cut with an endmill after the saw cut, then one more pass with the saw to clear the grooves, that should leave minimal burrs if the cutters register correctly (clean taper, good tooling and toolchange).
 
Last edited:
Thanks Milland. This is a job for myself a hobby project 18 cyl radial. Building it from a set of plans from Ageless Engines. Plans say it can be built in 2000 hours. Of course this is with manual mill with a rotary table and a 9 inch lathe. The part I am working on now they claim it takes about 5 hours each. 80 of them equals 400 hours. A friend with a job shop doesn't think most guys. Running a manual machine and a rotary table could get one done in five hours. Anyhow if I can get them slotted I should have less than 40 hours in 80 of them. Doing this project to learn to be faster with the machines that I have. I am doing this on a Bridgeport clone with a 2 axis Accurite millpower cnc.


The aluminum is 6061 t6511. Its what the plans call for. So yes kind of soft stuff. Plans call for the slitting saws I have. They are HSS 90 tooth .040 thick. After you posted I looked in the catalogs that have for some with less teeth and 90 was as coarse as I could find. Plans say to run the saw 600 RPM's and to use Johnson past wax. Was using alumnacut and Wd40 mixed for lube. Trying to keep the saw lubed and blowing the chips out. If running to fast or feeding to fast it wanted to plug the teeth up. Was running at 600 RPM's and 8 inches a minute. I will have to play with my technique and see that I can do.
 
Using a wax is begging to clog the teeth, so at least you're using a liquid of some sort. But you really need something to "blast" the clips clear of the teeth, which is why I recommended some sort of mist or flood cooling. Coarser cutters are available in HSS but you'll have to dig for them, and it might not be worth the time or money.
 
All good stuff from Milland's right, the wax just retains chips.

An alternative to coolant is air blast. Play with it to see where to direct it, and how much, how many nozzles. if running a circular path unattended, 4 nozzles are often needed to compensate for direction change.

FWIW, I use Loc-line with 1/8" nozzles, then 1/8" copper tubing through the nozzles, flaring the inner end a bit to keep it from slipping through the nozzle. Or buy the OEM nozzles, but they list at >$10 each.
 
Hey guys Your right about the wax. Tried some bee's way with and without a cutting oil. Plugged things up. I don't think there is enough heat generated during the cutting to keep the bee.s wax melted. So far Lube and a blast of air seems to work. If they are cut one grove at a time any way you want to cut them doesn't seem to be a problem. But is painfully slow. What do you guys think about the RPM and feed rate? Conventional or clime?
 
Climb for sure, tool speed seems OK, not sure on the feed.

If you're dead set on using wax, you can thin it with kerosene. We would pour some kero in a glass jar then use a torch to melt the wax into the liquid. Be careful, it may catch fire. After it cools it sets up as a paste, the kero/wax ratio determines its consistency.

I'd rig up a little water fall pump and direct some flow towards the cutters if for no other reason than to aid chip evacuation.
 
One thing WD-40 does well is act as a tool lube for aluminum on a B-port.
But you also need air to clear the chips.
Going back and forth with the spray bottle and the air hose while turning the handles is a dancing act to say the least.
Anybody tried putting WD-40 in a cheapo mist unit for such work? Even if the left hand has to move and point the nozzle into the work area.

I always try to climb cut in aluminum.
It's hard to get too many RPMs in al but then you need a feedrate to keep up so that you are milling and not grinding.
This limits the spindle speed.
For every cutter geometry and cut there is also a "no-mans" land where it chip welds. Slower makes it go away, higher makes it go away too.
On a B-port this chip weld is that not clean sound and a resistance in the handle.
Do not push through and break off the bad stuff on the tip, stop. ( I admit to not following this advice, sometimes ok, sometimes not)

Welded aluminum cutters if pulled at the first notice of oh-poop can be cleaned with phosphoric acid, naval jelly, toilet bowl cleaner, even coca-cola if you give it enough time.
High strength phosphoric while the nicest of most acids will attack and etch HSS so do not sit any longer than needed.
I can forget and leave carbide in such overnight with nothing. 10 minutes will kill a HSS drill designed for aluminum.

I digress and wander...
The WD-40 thing in aluminum cutting at B-port or small lathe speeds with carbide or HSS.
Bob
 
I would spin far faster in alu, i have acculube and the air blast clears things great, i use those little blades a fair bit, i think thoes are really aimed as screw head slotting, if build up is a issue, more speed less feed, run out is a issue with those blades, so i oftern find only a fraction of the teeth cut. if you have a good bench grinder with a nice rest, its really easy to just grind out every other tooth too. Never tried to cut any alu with them, everything i slot with thoes is free cutting steel or stainless. But yeah, a burr is part of the coarse, they never seam to have enough relief to cut clean and the full width chip does not help, stagger grind every tooth corner might go a long way to solve that too. just rerun your external tool and give it a wipe with some scotch brite and the little burr should nicely disappear is probaly the simple fix.

Had a job circa 40 thou too but only about the same 30 depth cutting groves in 6' long 304 stainless 4mm sheet, all done on the Bridgeport and lots of repositioning. Worse part of that job was the circa 400 hole vacume pattern the customer invented for it, took bloody ages!
 
Thanks for the replies. This is being done on a Bridgeport type machine(Sharp) with a 2 axis cnc. So I don't have to crank the handles. Would it be better to do it in 2 passes? The dept of cut is .050 and the dept of the teeth on the saw is less than that. When I get back on them I will get a video of the action to see what you think.
 
I would take two, or even more cuts with the final finishing cut to get a clean finish. Saws need be really sharp and some form of coolant important. Playing with the speed to get the best setting for the job. Slitting saws can crate a resonance at certain speeds. As well, I would make the spacers between the saws as large as possible, almost to the level of the cut.
 
Last edited:
.050 isn't much. Do it in one pass.

If the saw isn't tracking dead-on (likely), there'll be a ding where it reenters the cut. The fewer reentries, the fewer dings.
 
We sell HSS and carbide saw blades. 1-3/4" dia HSS screw slotting blades are standard with 64 or 90 teeth, carbide standard is 38 teeth. We can make other configurations, please speak to a salesperson.

May want to consider an alternate bevel, where 1/3 of every tooth is beveled, alternating left and right corners. This helps with chip clearance issues.

Compound land is another option to better clear chips.

Circular Saw Blade, Circular Saw Blades, Jewelers Saw, Saw Blades - Martindale
216-521-8567
[email protected]


HTH,
M
 
Mountie Thanks for the link, Could you tell me do you also have some kind of special spacers to use with saw blades. Looks like most blades are hollow ground. So would it be ideal to have special spacers to match up with the hollow grind . In my case I need 5 .040 saws spaced .040 apart. In my case I ground down some used saws for spacers . I think this can cause a problem because of the hollow grind. Also the stack hight and spacing is off . I think a stack made this way when clamped together is causing warping or distortion in the blades. What is your thoughts on making a proper stack of slitting blades.
 
Depends on the blade. Most hollow ground blades work best if used with a spacer. The spacer supports the saw over a larger radius than the arbor. The spacer must be small enough for your finish depth + some clearance.

Another option is blades with integral hubs. The hubs are ground flat and parallel, while the cutting section of the blade has side clearance (a.k.a. dish) for freer cutting. Precision hubs may also be used in lieu of spacers.

HTH,
M
 
Thanks again Mountie . Blades with integral hubs sounds like the hot ticket but at what price. On the normal hollow ground blades. A flat parallel spacer in different diameters would need different thickness to maintain the .040 spacing between the blades because of the hollow grind. Also will it make a difference that the blades will only be clamping on the thin outside edge of the spacers?
 
Climb cut with slitting saws on a bridgeport w/ rotab seems like asking for trouble, and those small teeth will pack off really fast if you're not careful with feed and DOC- a slow and consistent feed can be tricky by hand. Concur with desirability of coolant, particularly flood to help wash out the chips.

These saws in question are fairly thick so maybe not as big an issue, but with the thinner ones I usually only feed .005 or .010 on the first few passes to avoid distorting the cutter, once its in the cut about the depth of a gullet then I increase it a bit but never a lot more than the blades thickness.
 
Blades with integral hubs sounds like the hot ticket but at what price.
I work in the machine shop/engineering, so I've no idea. Contact sales (contact info above) for price/delivery.

A flat parallel spacer in different diameters would need different thickness to maintain the .040 spacing between the blades because of the hollow grind. Also will it make a difference that the blades will only be clamping on the thin outside edge of the spacers?
Since most blades only have a dish of .001/.002 per side, depending on OD, the spacing is solvable, depending on your tolerances. Call sales for details.


M
 








 
Back
Top