Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    pak's Avatar
    pak
    pak is offline Cast Iron
    Join Date
    Oct 2007
    Location
    Miami Fl, USA
    Posts
    364

    Default 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?
    I tried to post a picture of the part, but it said invalid thread.


    Regards,

    Drew

  2. #2
    Finegrain is offline Titanium
    Join Date
    Sep 2007
    Location
    Seattle, Washington
    Posts
    3,380

    Default

    .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.

    Regards.

    Finegrain

  3. #3
    Metalcutter's Avatar
    Metalcutter is online now Titanium
    Join Date
    Sep 2005
    Location
    San Diego
    Posts
    2,797

    Default

    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
    "fix".

    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
    result.


    Stan Dornfeld
    San Diego


    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.

    Best regards,

    Stan-

  4. #4
    gatz is offline Cast Iron
    Join Date
    Sep 2006
    Location
    Lincoln, NE
    Posts
    333

    Default

    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.

  5. #5
    pak's Avatar
    pak
    pak is offline Cast Iron
    Join Date
    Oct 2007
    Location
    Miami Fl, USA
    Posts
    364

    Default Follow up

    Quote Originally Posted by Finegrain View Post
    .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.
    At .001 IPT I should run 163 IPM. That sounds safe.

    MetalCutter,

    Thanks for the prompt response and the tutorial.

    Gatz,

    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,

    Drew
    Attached Thumbnails Attached Thumbnails transmission-lever-dscf2572.jpg   r-port-shaft-small.jpg  

  6. #6
    gatz is offline Cast Iron
    Join Date
    Sep 2006
    Location
    Lincoln, NE
    Posts
    333

    Default

    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.

  7. #7
    dp
    dp is offline Banned
    Join Date
    Aug 2005
    Location
    Puget Sound, Washington
    Posts
    3,204

    Default

    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.

  8. #8
    Hdpg is offline Stainless
    Join Date
    Feb 2009
    Location
    Vancouver, B.C. Canada
    Posts
    1,802

    Default

    Quote Originally Posted by gatz View Post
    ......however, 1/64 is very thin...........
    Yes 1/64 is very thin but .064 which is what was in the first post is not very thin.

    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.

  9. #9
    pak's Avatar
    pak
    pak is offline Cast Iron
    Join Date
    Oct 2007
    Location
    Miami Fl, USA
    Posts
    364

    Default Follow up

    Quote Originally Posted by gatz View Post
    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.
    The pin to which the clamping bolt clamps does not have a relief or a flat. However, it does have a ball that engages in one of three detents, one for neutral, forward and reverse. It is up to me to align the lever to the switch and gear cables.
    Quote Originally Posted by gatz View Post
    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.
    You are right, it is a non-critical cut. The saw that I will be using is slightly larger than 1/16th – about .0015 more. I thought this would be about right. If not, MSC has shipped already and I own it.
    Quote Originally Posted by gatz View Post
    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.
    Looks like you picked up on my personality pretty quick. The real reason for using a slitting saw is that I have already done a number of projects requiring the same type of slit using the band saw. The results were satisfactory, but like you said, I like things nice and tidy.
    Quote Originally Posted by dp View Post
    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.
    Good points to keep in mind. Thanks much.
    Quote Originally Posted by Hdpg View Post
    The speed and feed are just ridiculous; something like 800 to 1000 rpm and maybe 10ipm feed with lots of coolant should work.
    Your numbers look more like what I thought they should be, but I have never used a slitting saw and the Handbook only confused me. I don’t have a manual mill to test the feed, so I have to be right the first time. I suppose I could put a test piece in my lathe. Thanks for the numbers.

    Regards to all,

    Drew

  10. #10
    gatz is offline Cast Iron
    Join Date
    Sep 2006
    Location
    Lincoln, NE
    Posts
    333

    Default

    Sorry, mistook the .064 figure.

    That's a more realistic number for slitting something like the lever.

  11. #11
    Hdpg is offline Stainless
    Join Date
    Feb 2009
    Location
    Vancouver, B.C. Canada
    Posts
    1,802

    Default

    You are not in a hurry; go even slower like 600rpm and a feed of 2ipm to start, the key is lots of coolant.

  12. #12
    bronto48 is offline Hot Rolled
    Join Date
    Apr 2006
    Location
    Laytonsville, Maryland
    Posts
    533

    Default

    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 06:12 AM. Reason: add comment

  13. #13
    Conrad Hoffman's Avatar
    Conrad Hoffman is online now Stainless
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    1,668

    Default

    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.

  14. #14
    Hdpg is offline Stainless
    Join Date
    Feb 2009
    Location
    Vancouver, B.C. Canada
    Posts
    1,802

    Default

    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.

  15. #15
    pak's Avatar
    pak
    pak is offline Cast Iron
    Join Date
    Oct 2007
    Location
    Miami Fl, USA
    Posts
    364

    Default

    Quote Originally Posted by gatz View Post
    Sorry, mistook the .064 figure.

    That's a more realistic number for slitting something like the lever.
    gatz; There is no need to appologize. There is an old saying that I believe in my heart. "A man who makes no mistakes makes nothing." For this reason, I have become a master of disguise.
    Quote Originally Posted by Hdpg View Post
    You are not in a hurry; go even slower like 600rpm and a feed of 2ipm to start, the key is lots of coolant.
    I have nothing scheduled for the next forty years. It takes me more time to respond to these posts than it would to cut at 2ipm. Slow is better. Thanks for the advice.
    Quote Originally Posted by bronto48 View Post
    Feeds are s-l-o-w...Depth of cut around 0.10 to 0.15 inch. Shallower cuts present less problems than full depth cut....Spindle speeds are in range of 300 to 600 RPM for diameters mentioned...It is a slow process. 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.
    I get the feeling that slow, shallower and slow are the key theme when slitting. With regards to "design", I find it rather interesting. I will keep it in mind for my next project.
    Quote Originally Posted by Conrad Hoffman View Post
    I use these quite a lot on my (yecch) manual mill drill with no trouble...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.
    Conrad, "yecch" sounds like you don't like your manual mill. IMHO, if I had started on a [yecch], I probably wouldn't be asking these 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.

    Quote Originally Posted by Hdpg View Post
    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.
    I have an arbor that Chin Wan Q made. I hope his slanted view on life does not translate to his arbor.

    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.

    With respect,

    Drew Keyes

  16. #16
    67Cuda's Avatar
    67Cuda is online now Titanium
    Join Date
    Oct 2008
    Location
    West Coast, CA
    Posts
    2,205

    Default

    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.

    Tom

  17. #17
    willbird is offline Banned
    Join Date
    Jul 2005
    Location
    North(very) West(very) Ohio...near exit 13 on OH turnpike
    Posts
    3,714

    Default

    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

    Bill

  18. #18
    Conrad Hoffman's Avatar
    Conrad Hoffman is online now Stainless
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    1,668

    Default

    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.

  19. #19
    metlmunchr is offline Diamond
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,285

    Default

    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.
    Attached Thumbnails Attached Thumbnails clamp-bolt.jpg  

  20. #20
    rockfish's Avatar
    rockfish is offline Titanium
    Join Date
    Aug 2006
    Location
    Munith, Michigan
    Posts
    2,013

    Default

    We do an awful lot of saw slitting at our shop and I will have to agree that slower is better. At speeds above 600 RPM, you're going to run into trouble I think.




    Frank



    www.randolphmach.com

Page 1 of 2 12 LastLast

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •