Results 1 to 20 of 25
Thread: Slitting Saw Feeds and Speeds
06-24-2009, 01:00 PM #1
Slitting Saw Feeds and Speeds
I will be using a HSS 2 ¼” diameter x .064” thick slitting saw on a CNC mill to cut aluminum. I have three questions.
- How many teeth should the blade have – 132 or 60? I haven’t bought it yet.
- I have studied the Handbook and have no clue about how to translate the information into useful terms?
I will be using Case 2 in Fig. 5 on page 1043, as in cutter feed parallel to the surface of the work piece, as in slotting or side milling.
From Table 11, I find that SFPM should be 1600 and Feed should be .016/tooth.
From my calculations, that would be 2714 RPM for a 60 tooth saw @ 2605 IPM.
That feed sounds mighty fast to me – even at half that rate.
Simply put, what is a safe speed and feed for this operation?
- Can I cut to full depth (5/8”) in one pass or should I cut in multiple passes? If multiple passes, how deep should I go for each pass?
06-24-2009, 01:08 PM #2
.016" per tooth seems like a lot, and I should think you will break the cutter very quickly owing to clogging of the gullets and subsequent galling and heating. I'm guessing more like .001" per tooth. You do want the RPM's up high enough to blow the chips well clear of the cutter.
06-24-2009, 01:26 PM #3
The Slitting Saw and the Woodruff Cutter
Slitting saws and Woodruff cutters work in much the same way; so we
can just call them saws for now. Saws have one big difficulty.
After we understand that difficulty we will solve it and increase
their performance. First a little background.
After you dig a hole in the ground to fix a water pipe you need to
put the dirt back. However all the dirt wont go back because it
doesn't fit anymore. The dirt has been "upset". That is, all the
little grains of soil and pebbles are no longer nestled together in
a compact form. This upset condition also happens in metal during
the cutting process.
Upsetting the metal increases its volume. So the metal in a chip
that is cut from a bar takes up more space after it has been cut.
Parting off steel in a lathe using a slender "part off" tool
creates a long slender upset chip. This chips volume is greater
than when it was compact material in the parent metal. And greater
also are its dimensions. The chip is longer, thicker and wider.
The wider condition is what causes the problem. The kerf or groove
being cut has a width as wide as the part off tool. During the
cut, the emerging chip is actually wider than the groove being
formed. So the chip is in the groove under a "press fit"
condition. As the bar is rotated the press fit chip is being
forced down against the cutting tool. The tool has to support the
pressure of the downward cut in addition to the downward force
created by the emerging chip. The deeper into the bar the tool
cuts the greater these forces multiply; because the chip grows
longer before exiting the groove. The tool will break during this
process unless the cut is shallow or the feed rate is very light.
A light feed rate will create a very thin "ribbon" like chip with
light forces; but this takes a much longer time to do the work.
The difference between a part off tool and a slitting saw is a
slitting saw has many "part off tools" or teeth around its axis.
Manufactures of these saws make them with tooth forms which have
flat ends on the teeth like a part off tool. These teeth then cut
a chip which is as wide as the slot just like the lathe tool and
with the same problems of high destructive forces caused by the
"press fit" chip being formed. Unlike the lathe tool the saw has
many teeth. So if one tooth misses cutting something the tooth
coming right behind it can scoop up the remainder. Now to the
A double cut saw blade has chamfers on alternate teeth. These
chamfers on one corner of the tooth are made by grinding away one
third of the tooth on the left side of the first tooth and then on
the right side of the next tooth and so on. This grinding is done
on each tooth at a 45 degree angle. Now when the saw cuts, it cuts
a chip on the left and then a chip on the right. These chips are
only two thirds as wide as the slot. The following tooth has its
chamfer on the other side and so it picks up the remainder of what
the first tooth left. The forming chip isn't wide enough to rub
both sides of the slot so the slitting saw can cut very freely and
take a heavier chip load. Higher production can then be the
As the years have gone by I've learned a few more things.
The chip load can be pretty good if the tool has the chamfers.
The rule of thumb is "three teeth in the cut." One entering, one working, and one leaving.
Get the tool with the least number of teeth for your job.
You can get along with more teeth in the cut just don't push it. If you are interested in finding out something, use the cutter first in a hand mill and feel the difference between un-chamfered teeth and when they are chamfered.
06-24-2009, 01:31 PM #4
How many parts?...What length of cutter engagement?
Slitting or slotting saws seem to work better when taking full depth, however, 1/64 is very thin. Maybe take 4 passes, first one being somewhat shallow to establish the cut.
Is this width mandatory?, or can it be made wider; say 1/32 or more? Thicker the slitting saw, the less trouble you'll have. Make sure the arbor is supporting the cutter sides as far as it can.
Also, if you've got a LOT of parts to run, you might consider using a "roughing" cutter that is only using a portion of the cutter, say 1/4" max depth of cut; the rest being held firmly by an arbor suitably made. You'd end up with (at least) 2 cutters, but it may be worth the trouble.
Go with the 60T. Yes, the feed/tooth sounds high.
You might start at about 1/2 of both the suggested Speed and Feed to see how it goes.
Use flood coolant.
06-24-2009, 01:55 PM #5
Thanks for the prompt response and the tutorial.
I will only be making two of these parts. They will replace my 3208TA Cat/Twin Disc shift levers in my boat. They will also serve as a roller to actuate nuetral cut-out switches to prevent a start in gear. I was able to upload the pictures this time.
Although the width is not critical, I wanted this thickness for several other projects as well. You can see from the pictures where the slot will be. I will be using flood coolant and take it in multiple passes as suggested.
Best Regards to all,
06-24-2009, 08:48 PM #6
Can't quite tell from the pic, but does the clamping bolt align with a small relief-cut in the shaft that it's mounted on?
If so, that would ensure correct engagement to whatever is inside the drive.
This type of slit is non-critical; just needs to be of sufficient width so that when the bolt is tightened up, that the 2 "ears" don't collapse against each other and prevent the lever from actually tightening up on the shaft. And for this application, 1/64 seems small indeed.
Whatever clearance has been provided between the shaft and the hole in the lever will be a factor. If it's too loose a fit, you're going to have the "ears" hitting each other before the clamp gets tight.
With your other projects in mind, I'd definately give thought to going to a wider cutter.
Also, I realize you'd like things to be neat and tidy, but scribing a line at the intended location and using a hacksaw to make the cut would be far more economical and take less time. If you're concerned about making a straight cut, just clamp some sacraficial pieces of steel alongside the scribed line (half the blade thickness & front and back)...then when cutting, kinda favor that side. The steel pieces will definately help.
You could also do this in a vertical metal bandsaw.
06-24-2009, 09:03 PM #7
A characteristic of circular saws that I have used for slitting is that only a very small part of the saw ever touches the work. Like maybe 30 degrees of the circle. This is because of errors in the saw, arbor, and quill. This affects the rate at which metal is removed. The other thing I found is that if the arbor is not perfectly 90 degrees to the direction of travel the blade will quickly walk off the desired line and break. I had the best results using lots of passes of no more than 0.010 DOC.
06-24-2009, 11:08 PM #8
The speed and feed are just ridiculous; something like 800 to 1000 rpm and maybe 10ipm feed with lots of coolant should work.
But as was pointed out a bandsaw cut will be perfectly adequate.
06-25-2009, 05:32 AM #9
Regards to all,
06-25-2009, 05:52 AM #10
Sorry, mistook the .064 figure.
That's a more realistic number for slitting something like the lever.
06-25-2009, 06:01 AM #11
You are not in a hurry; go even slower like 600rpm and a feed of 2ipm to start, the key is lots of coolant.
06-25-2009, 07:04 AM #12
I often use same and smaller diameter but thinner (0.020 down to 0.010 inch) slitting saws when working aluminum on my all-manual Clausing mill.
A few observations, based on the feel of the x-axis crank and such:
Flood cooling is necessary to sweep out/unclog chips, otherwise it just loads up and stops cutting. Crooked kerf and breakage soon follow.
Feeds are s-l-o-w, otherwise the saw loads up/breaks or wanders off the cut direction.
Depth of cut around 0.10 to 0.15 inch. Shallower cuts present less problems than full depth cut. Heavy depth of cut also seems to risk cutter wandering off from straight cut, feeds become very slow due to chip/loading issues.
Spindle speeds are in range of 300 to 600 RPM for diameters mentioned.
Off center spindles/runout seems to be a way of life for slitters.
It is a slow process.
When it all works, results are terrific.
Have spare slitters on hand, just in case....
Opinion (not an observation):
Cutting slot with band saw and cleaning up kerf with slitter risks slitter following crooked kerf if feed is too fast. Go slow. I have not yet tried this technique.
On edit: I find it fun to "design" (trial and error) my clamping slots so that when the clamp bolt is fully tightened, the slot completely closes and disappears but adequate clamp force is realized. Makes for a very neat looking job.
Last edited by bronto48; 06-25-2009 at 07:12 AM. Reason: add comment
06-25-2009, 10:37 AM #13
I use these quite a lot on my (yecch) manual mill drill with no trouble. 1000 rpm should be no problem. Use a very light coolant- I actually like WD-40 for some things, rather than oil, because the chips fly off more easily. It's very easy to dish a thin saw if your arbor is junk, so do up a proper arbor on the lathe that contacts the blade in a defined area and has a cup type cap to match. It should run as true as possible- there's no reason to have partial contact around the saw. Mine cut over 360 degrees and make the same sound all the way 'round. I typically saw full depth regardless of what it is. I'll slow it down for very deep cuts. I use a loose rule for speed- if the number of teeth and speed make for an annoying tone, I slow down. One more thing- be sure *both* sides of the saw are getting coolant.
06-25-2009, 10:49 AM #14
If you are making your own arbor do the final turning for the boss diameter and the face in the milling machine to make sure it is running as true as possible.
06-25-2009, 02:22 PM #15
neophyte questions. At least you have a feel for what you are doing. With CNC, you have no feel. You have to ask guys like you for advice. I get the slow down theme, but you have hit on something that no one else has - coolant on both sides of the blade. Fortunately, I have two outlets. Great info, thanks.
I am truly amazed at how much one can learn from this forum. I can’t wait to find a way to contribute in some small way. Thank you all.
06-25-2009, 03:14 PM #16
Line up the slitting saw center line of your part and feed in to full depth of cut @ 300-400 rpm keeping cutting oil/coolant on it, then bring it out and take one full depth conventional cut. You'll feel and hear what the cutter wants in either feed or speed. Adjust each accordingly.
06-25-2009, 03:56 PM #17
I have used a lot of 1.5" woodruff slitting saws. On CNC equipment, once you make a few parts by machining them then slicing them off of the extra stock still clamped in the vice you will get addicted to the process and use it a LOT.
I used them on A2, O1, 4140HT, M42, S7, 6150, and many other ferrous and non ferrous materials. I typically used the same SFM I would use for any other HSS tooling in that metal, and fed them .001 to .002 per tooth, typically I climb cut around the parting using the same profile program I milled the perimeter with (programmed for a 0 dia cutter and using the tool dia as a Dia offset). With a 1.5" cutter I usually used about a 1.4" offset if that would work out.
I broke very few of them, almost none in fact.
Most of the time I ran them in a 1" dia extension held in a 1" straight shank holder, gripping the 1/2" shank by a flat ground at the rearmost portion of the shank. The resulting surface finish was good enough to be a finished part.
For very thin parts (in the Z direction) you could often run several off the same block of material before loading another one.
For a 1 off or 2 off job you will not gain anything by trying to run the SFM up at the upper end of what is possible, the setup time far outweighs the cycle time in cut.
Also keep in mind that the part might want to close up on your saw due to stresses built up from the prior machining
06-25-2009, 06:20 PM #18
Drew, I have to say "yecch" when I mention my Grizzly mill/drill. This forum is populated with well equipped professional machinists and once I mention mill/drill, I suspect all credibility goes out the window unless I dis the thing a bit. I'd love a real mill, but space, money and WAF hold me back. Actually I can make rather good parts on it, though I attribute that more to the good Kurt vise holding the mill solidly on the stand.
07-08-2009, 01:46 AM #19
Drew, the attached sketch shows a clamp which works much better for aluminum than a slotted pinch arrangement, and gets right on up there on the neat 'n tidy scale too.
Semi circular cutout depth in clamp bolt is equal to the amount you'd overlap the cross hole with the mounting hole, and its radius is equal to the radius of the stud you're going to mount your part on. About .05 to .06 depth for a 3/8 clamp bolt.
Clearance drill the half the bolt passes thru. Drill and tap the other half for the sockethead capscrew. #10 screw will work with 3/8 clamp bolt.
Crosshole in arm drilled to match clamp bolt diameter. Can be drilled thru or blind as shown. Length of the clamp halves can be adjusted such that the head of the screw is down inside the hole.
07-08-2009, 02:43 AM #20