584,871 active members*
5,364 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Tormach Personal CNC Mill > Cutting a 7.1" circle from 0.5" thick 6061 alum - End Mill "loading up"
Page 1 of 2 12
Results 1 to 20 of 22
  1. #1
    Join Date
    Mar 2009
    Posts
    75

    Cutting a 7.1" circle from 0.5" thick 6061 alum - End Mill "loading up"

    I have a PCNC 1100 that I use in my Fabrication shop for various internal work.... don't really advertise or "hire out" with it (because I am not proficient with it).

    A friend was in a bind, and needed some tools made to press some bearings.... He needs two circles cut from 0.5" thick aluminum... one circle 7.1 inches and one circle 7.4 inches.... sounded easy enough...... I ordered the material online (8" x 8" squares)..... I ordered twice as much as needed so that I could screw up.

    .... I struggled with feed and speed for a while.... finally I dialed it way back to what I thought was a safe setup... just so I could get it done..... (broke a few end mills)......

    In the end, I was using a .25" end mill.... running at 3" per minute, taking a 0.05" bite..... this worked well until I got down to about 0.35" ~ 0.4" deep... the end mill started "loading" up on me.... the flutes would fill up (packed) with aluminum.... the first couple of times this happened I didn't get shut down in time and the end mill broke.... eventually I got to where I could here the motor slow down, and stop it before it broke....

    I am theorizing that the reason that it was loading up, was that I was so deep in the cut, with both metal against both sides of the cut.... can someone please give me some pointers of how I should have set this up?

    .....

    By the way.... I did actually get the 7.1" completed..... I was so close to getting it.... I was cut through 0.45" of the 0.5" .... only 0.05" to go.... but it finally got to where I could only move about 1" and was loaded up..... and each time I would load up, I had to hit the e-stop..... that seemed to make my x and y co-ordinates lose steps (cause when I would re-start, the cut would be ever so slightly off).

    So, I took the 8" x 8" out of the vise.... and "broke" the outside off (leaving me a circle that had rough edges on the top .07" or so... and a few other rough spots....... then I chucked it up in my 4th axis (mounted horizontal).... brough the end mill to the edge of the material...and turned the 4th axis... was able to clean it up pretty nicely.

    - One thought I have for the 7.4" piece is a bit off the wall..... I have a cnc plasma table, and I was thinking of cutting it a bit oversize say 7.6" circle... then chuck that in my 4th axis and spin it down to the prescribed 7.4" ..... I know that it not the correct way to do it... but the experience tonight had me ready to pull my hair out.....

    Look forward to suggestions and advice.

  2. #2
    Join Date
    Aug 2007
    Posts
    92
    2, 3 or 4 flute cutter? whatever the case, your feed is very slow. I'd be running a 1/4 2 flute tool around 5000 and a bit over 300mm/min with coolant. Ideally a bigger tool would do a better job, I use 12mm slot drills for everything I can, they're a nice balance between metal removal and HP use.

  3. #3
    Join Date
    Jan 2013
    Posts
    306
    Are you using any coolant? Or air to keep chips removed?
    3ipm is really slow. I cut at 8,000 rpm 30ipm .040 DOC without any problems 2 flute carbide.
    Use a little wd40 and air to keep the chips cleared.


    Sent from my iPad using Tapatalk HD

  4. #4
    Join Date
    Jun 2008
    Posts
    1082
    I am by no means an expert so take my answer with a grain of salt...

    Did you use anything to calculate the feed and speed? It seems like 3 IPM is extremely slow. Also, 50-thousandths is pretty shallow for such a powerful machine like the PCNC 1100. I think that's the depth of cut I used to use on my TAIG (which is a very small mill). With such a slow speed and low depth you're basically creating aluminum dust. Heavier chips might have enough inertia to fly clear of the cut but the dust will probably just settle.

    I guessing proengines' speed of ~12 IPM is what he or she would do with a full-depth slot. To say it another way: IF proengines IS recommending ~12 IPM for a full-depth slot: it would cut 40 times faster than what you're doing now. (10 times deeper at 4 times the speed)

    Also, are you using coolant? Although I haven't used it myself, I've seen a lot of people recommend WD-40, even over specialty coolants.

    Check out FSWizard. I'll attach a pic of the page where it's recommending 5000 RPM @ 18.2 IPM for the numbers I plugged in. (0.25" 2-flute HSS cutter doing a 0.17" slot in 6061)
    This speed and feed will cut your circle about 20 times faster.
    Attached Thumbnails Attached Thumbnails 0.25x0.17.png  

  5. #5
    Join Date
    Jun 2008
    Posts
    1082
    Here's a video showing a Tormach PCNC 1100 doing some cutting in 6061 with a 1/4" end mill.

    This guy records a lot of really good videos! If you're interested in using your machine more you could probably get a good idea of what you can do by spending a few hours watching the videos.

    https://www.youtube.com/watch?v=I0MVFvLlOQI

  6. #6
    Join Date
    Feb 2006
    Posts
    7063
    Having the tool load-up is a clear sign of either way too much RPM or way too little feed, which makes the tool heat up, resulting in chip welding. With a 1/4" tool, you should be running max RPM, and should by up between 15-20 IPM. Depth can be whatever the spindle can handle - easily 1/2 the tool diameter. Ideally you should have coolant, but can probably get away with just an air blast to keep the chips clear. Use only a 2 or 3-flute in 6061. The chips should be coming off HOT, and the tool should remain cool, with no welding.

    Regards,
    Ray L.

  7. #7
    Join Date
    Dec 2012
    Posts
    59
    Here are the obligatory Gwizard numbers, while making some assumptions about your tooling and setup. Be aware that when slotting in aluminum, particularly with deep cuts, chip removal is hugely important. Flood cooling or a strong airblast is assumed.

    So,
    Tool = .25" HSS two flute cutter sticking out .6" and Material = 6061 T6
    Depth of cut = .125" (I picked this as my user controlled variable; 1/2 tool diameter is my sort of default and happens to give reasonable numbers here. You could monkey with this to improve MRR or reduce tool deflection)
    RPM = 5100 (max for the 1100)
    Feed rate = 18.4 IPM

    These numbers are highly dependent on stickout, tool material and flute count. The one caveat is that I prefer not to run at full spindle speed; it's just noisey and I'll accept a lower feedrate in exchange for less noise in my small shop and operating nearer the motors peak power point. Personal preference for a cut like this.

    No matter what, 3ipm is way too slow. I know you're trying to baby the cut but your problem here isn't going too fast, it's going to slow and/or using a tool with too many flutes. Increase your RPM, Feed and reduce the number of flutes while you're at it. Reducing flute count will accomplish two really important things; it will provide more room for the chip to clear out of the cut and allow you to run at 15-25IPM feed rates while maintaining chip load. Remember that the more flutes you have the faster you must feed in order to keep an adequate chipload; a four flute cutter would need to go 36ipm for the same cut to stay happy. The machine is capable of that, but you'd have problems with chip packing in short order.

  8. #8
    Join Date
    Mar 2009
    Posts
    75
    Thank You everyone for the good advice and info!!! I see that I have made several mistakes.

    I was using a 4 flute cutter (most of the time)....... it is what I had......

    at times I tried 1/8", 3/16", 1/4" ...... (all because that is what I had).....

    Coolant - I had a shop vac up right next to the spindle and it seemed to be doing a really good job of removing the chips....

    - I was running at th max 5120 rpm's....

    ---- again, thanks for all the quick ... good input....

  9. #9
    Join Date
    Mar 2009
    Posts
    75
    One other thing to mention..... I will have a problem with the 7.4" circle (the one I still have to cut)... that I did not have with the 7.1" circle......


    The material I have is 8" x 8" .... so, with 7.4" of part.... and using a .25" end-mill .... leaves me at 7.9" ...... the material actually is about .125" oversize... so a little relief there.... but I will be "tight" getting the tool between the vise jaws on the front and back without touching them.....

  10. #10
    Join Date
    Feb 2006
    Posts
    7063
    Quote Originally Posted by herrmc View Post
    One other thing to mention..... I will have a problem with the 7.4" circle (the one I still have to cut)... that I did not have with the 7.1" circle......


    The material I have is 8" x 8" .... so, with 7.4" of part.... and using a .25" end-mill .... leaves me at 7.9" ...... the material actually is about .125" oversize... so a little relief there.... but I will be "tight" getting the tool between the vise jaws on the front and back without touching them.....
    What is going to be holding the part on the last passes?

    Regards,
    Ray L.

  11. #11
    Join Date
    Mar 2009
    Posts
    75
    Quote Originally Posted by SCzEngrgGroup View Post
    What is going to be holding the part on the last passes?

    Regards,
    Ray L.
    ...
    Ray,
    I worried quite a bit about that last night (while cutting)..... at first I had it configured so that I had 0.02" left as my last pass... and I wondered if that would be enough to hold the part.... and then I could just break it out?.. and then put it in the 4th axis with a taper bit and put a slight bevel on the corner to remove the ragged edge.....

    As I worked, I figured out how to use the "tabs" in my CAM s/w (Sheetcam)...... at the end of my exercise I had programmed in a tab on the front and back that was .125 tall and .25 wide ..... As it happened..... I gave up when I was at 0.45 ...... I took the part out of the vise and broke off the outside.... then, I put it in the 4th axis and removed the burr where I broke off the last 0.05" ....

    I am guessing that all of my approaches have better alternatives, and look forward to hearing how to do it correctly....

  12. #12
    Join Date
    Dec 2012
    Posts
    59
    Quote Originally Posted by herrmc View Post
    ...
    I am guessing that all of my approaches have better alternatives, and look forward to hearing how to do it correctly....
    There's probably a dozen ways to do this, and which is 'better' probably depends on a lot of variables. The real answer is whatever option gets you the part you want, and since there's more than one there's no correct answer.

    I'd probably opt to hold the stock on the table using toe clamps and a sacrifice plate underneath it. You'd be able to hold the plate down at its corners which should give you plenty of room between the tool path and the work holding. I'd then do my 2d profiling while leaving a couple of tabs, perhaps .050" tall and wide at their thickest. After milling, break/cut the circle out and smooth the edge either on the 4th axis, lathe or by file.

    An alternative to the tabs is, if it's tolerable, to put holes in the part you're cutting out and bolt/screw it to your sacrifice plate. That will hold the circle in place after it's cut free of the remaining stock, which is handy as you can now run a finish pass or what have you without worrying about breaking down your setup and having to find the center of the part again.

  13. #13
    Join Date
    Mar 2009
    Posts
    75
    Ok, I have looked through my pile of end-mills and I have a few .25" 2 Flute .... "Bosch 85911m" .... looked it up and says they are solid Carbide.

    - I have removed my vise and 4th axis, and have the material clamped directly to the bed on four corners (well, close to the corners)....

    - I have .125" spacers under the material to keep it off of the bed, and keep me from hitting it with the end-mill....

    ..............

    - I am not right away familiar with the term "stick out".... but it sounds very logical... how far the tool is "sticking out" of the chuck??? .... Mine is sticking out 1.375" from the bottom of the chuck...... I can push it up farther.... but i have two concerns...

    1.) it brings the chuck down where it might hit my work clamps...

    2.) I have pushed it into the chuck as far as the solid part of the shank goes....if I push it further, it will be on the spiral portion of the tool....

    ..... as sated before, the material is 8.120" x 8.120" x 0.5" ....... I need to cut a circle 7.4" ...... so with my .25" end mill, will be very close to the edge....


    I am going to try for a .12" depth of cut @ 12 IPM ..... I will have the Air hose standing by for cooling and blowing the chips out.....

  14. #14
    Join Date
    Mar 2009
    Posts
    75

    Picture of it mounted...

    I don't have proper hold down clamps.... but I think that these bolts and washers should work?

  15. #15
    Join Date
    Jan 2013
    Posts
    306
    A little cutting fluid of some type will help also. Wd40 works well.
    You did not mention RPM what speed are you planning to run?

    Spinning your stock will allow you to clamp further on the corners. Does not need to be square on the table since you are cutting a circle.

    Steve

  16. #16
    Join Date
    Mar 2009
    Posts
    75
    I may have forgot to mention my spindle speed..... I figured I would set it at the max of 5,120 .... should I slow it down a little?

  17. #17
    Join Date
    Mar 2009
    Posts
    75
    Dudes!!!! ---- Thank you all so much...... did in 10 minutes much better than we worked 4 hours last night!!!...... worked awesome.....

  18. #18
    Join Date
    Jun 2012
    Posts
    111
    When you say chuck, do you mean collet?

  19. #19
    Join Date
    Dec 2012
    Posts
    59
    Quote Originally Posted by herrmc View Post
    Dudes!!!! ---- Thank you all so much...... did in 10 minutes much better than we worked 4 hours last night!!!...... worked awesome.....
    Outstanding! Nothing quite as satisfying as getting a job dialed in and hearing your mill hum along making chips like it designed to.

    Couple points:

    Quote Originally Posted by herrmc View Post
    I am not right away familiar with the term "stick out".... but it sounds very logical... how far the tool is "sticking out" of the chuck??? .... Mine is sticking out 1.375" from the bottom of the chuck...... I can push it up farther.... but i have two concerns...

    1.) it brings the chuck down where it might hit my work clamps...

    2.) I have pushed it into the chuck as far as the solid part of the shank goes....if I push it further, it will be on the spiral portion of the tool....
    You're correct that stickout is defined as the length of the tool extending outside the tool holder. The longer the stickout the deeper into material you can cut, like the bottom of a deep pocket. The shorter the stickout the more rigid the tool. So you want the stickout to be as short as possible for the job at hand; it has a huge influence on how fast you can run the tool and quality of the cut.

    A limiting factor to stickout is indeed flute length. You can choke up on a tool in a holder till you reach the flutes but no further. So all tools have some designed in stickout that you can't get around. It's common to have a couple different lengths of each common tool size so you can match the length tool you need for a particular geometry. It's a little scary using a tool that puts the tool holder right over the top of the material at first, but you do get used to it.

    I don't have access to my F/S calculator right now, but the difference that 1.375" of stickout and say .75" would have on the cutout would be pretty significant, as would the difference between carbide and HSS.

    Quote Originally Posted by herrmc View Post
    I may have forgot to mention my spindle speed..... I figured I would set it at the max of 5,120 .... should I slow it down a little?
    RPM, Feedrate, cut width, cut depth, stick out, tool material etc. are all linked values in the feeds and speeds math. You can vary any of those parameters, but they'll change the others. So you don't have to run at any particular RPM. You could, for instance, run the spindle at 3000 RPM instead, but you would need to reduce feed rate to reduce the resulting chip load. For this kind of cut the limiting factor for material removal is probably going to be spindle RPM so running at max RPM gets you the fastest cut, but that isn't necessarily ideal (noise, spindle bearing wear, setup rigidity etc.).

    I would strongly recommend you invest in a feeds and speeds calculating software. It'll let you play around with these parameters and see how they influence eachother. There are a lot out there, but Gwizard is highly regarded. You can even buy it from Tormach, though I don't really understand what the advantage of that is vs. buying right from cnccookbook.com.

    Quote Originally Posted by herrmc View Post
    I don't have proper hold down clamps.... but I think that these bolts and washers should work?
    You're setup looks good to me. It's hard to argue with results. The use of the steel bars to balance the washers to is a good call. I like to use a full plate under my work, a 'sacrificial' plate, that I can cut into without worrying about. It fully supports the work piece and gives you a place to bolt the part to or what have you.

  20. #20
    Join Date
    Sep 2012
    Posts
    255
    Yep, tool stickout is the distance from the holder to the tip of the tool.

    It is importsnt to remember that manufacturers list cutting parameters for "ideal" length of their tools.
    It varies from one to another, but normally their stickout is only 2.5 diameters of the cuter.

    So a 1/4" endmill should only stick out 5/8" out out of the holder. Such 2 flute carbide endmill can slot aluminum at 0.25" depth of cut.
    If longer endmiil is used, depth of cut needs to be reduced by quite a lot.
    When you increase length of the cutter twofold, depth of cut needs to be reduced eigthfold if you want to keep the same deflection.
    Of cource often you want to sacrafice a little deflection and still run it deeper, thats when you get into trouble.
    In order to run deeper, you end up reducing feedrate.
    But cutter needs a proper chipload to work efficiently.
    In your case you reduced the chipload to the point of rubbing.

    So the rule of thumb is: NEVER compensate for extra length by reducing feedate.
    Always reduce the depth of cut first.

    Also check out my HSMAdvisor. It will help you figure stuff out.
    http://zero-divide.net
    FSWizard:Advanced Feeds and Speeds Calculator

Page 1 of 2 12

Similar Threads

  1. X Axis "Goes Off Pattern", "Awry", "Skewed", "Travels"
    By DaDaDaddio in forum Laser Engraving / Cutting Machine General Topics
    Replies: 1
    Last Post: 05-06-2013, 09:59 AM
  2. Replies: 8
    Last Post: 03-24-2013, 01:13 AM
  3. Replies: 5
    Last Post: 09-12-2012, 03:09 PM
  4. Replies: 1
    Last Post: 01-14-2011, 04:43 AM
  5. What's the best 1/8" end mill for 6061 alum.
    By Cycle Start in forum Uncategorised MetalWorking Machines
    Replies: 10
    Last Post: 03-19-2008, 02:34 AM

Tags for this Thread

Posting Permissions

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