584,841 active members*
4,264 visitors online*
Register for free
Login
Page 5 of 6 3456
Results 81 to 100 of 101
  1. #81
    Join Date
    Apr 2006
    Posts
    76
    Quote Originally Posted by BobWarfield View Post
    Fewer flutes can be thought of as decreasing spindle speed. This is important to the router folk, who often can't turn the spindle slowly enough with harder materials. Hence the one flute endmill was created for just such an audience.
    So let me get this straight, the one flute end mill is designed for routers because they cannot run their spindles slow enough?

    The reason for the single flute end mill is that they cannot get the feed rate high enough to get the chip load where it needs to be to prevent the flutes from clogging. The way you describe it is just confusing.

    You need to be very careful about advising people to slow their feed rate in aluminum. Slow feed rates in aluminum lead to BUE and flute clogging. You have to maintain the chip load to prevent this.

  2. #82
    Join Date
    Apr 2006
    Posts
    76
    Quote Originally Posted by BobWarfield View Post
    +1 on the 3 flutes--they effectively multiply spindle speed by 1.5 vs a 2 flute. BTW, when profiling and there's plenty of chip clearance, you could even try a 4 flute (yep, even with aluminum).

    Get chipload as low as you can go--I use 20% of mfg's recommended as my lower limit. If you go too low, the cutter will rub, which can give a great surface finish but is hell on cutter life.

    BTW, some fellas swear that running the endmill backwards is the ticket for burnishing aluminum profiles to a nice finish. Be sure to use an old endmill you don't care for too much though.
    Once again you confuse spindle speed with feed rate. A 3 flute increases your feed rate by 1.5, the spindle speed remains the same. I run 4 flute in aluminum all the time.

    I do not agree about the chip load. As you approach the max SFM (around 3000 in aluminum), decreasing the feed rate can destroy an end mill in fractions of a second. This is why it is so hard to prove out a program when you have a lot of RPMs to play with. You have to reduce the RPMs when you reduce the feed rate.

    If you cannot get a nice surface finish in aluminum using regular old end mills, there is a larger issue. Obviously the work holding method is the primary factor in this example.

  3. #83
    Join Date
    May 2005
    Posts
    2502
    Quote Originally Posted by UWP_Wes View Post
    I do not agree about the chip load. As you approach the max SFM (around 3000 in aluminum), decreasing the feed rate can destroy an end mill in fractions of a second.
    UWP_Wes, why does reducing the feed rate destroy the end mill in fractions of a second? Is no reduction at all possible, or is there something more at work here?

    My answer is that there is a particular phenomenon the governs how far you can reduce the feedrate. It's pretty straightforward to understand, and very quantifiable. It behaves the same regardless of surface speed, however, the cutter will fail faster if you're already at the surface speed limit because it will overheat, soften, and dull the edge that much faster.

    You only need to maximize chipload to maximize MRR's. The sweet spot for surface finish will involve somewhat less chipload. The lower limit of chipload is a function of the radius of the cutting edge. That's not the radius of the tool, but the radius of the edge itself if highly magnified.

    Here are the two cases:



    The top one has a chipload > edge radius. Lower one has chipload less. Top one shears through the cut by getting the edge radius under the chip, while the bottom one has to scrape the material. That's what's referred to when machinists talk about running too slow and "burnishing" or "rubbing".

    And yes, it will dramatically increase BUE in aluminum if you get close to this chipload range. You can see pretty graphically why from the drawing. The lower image is practically inviting the aluminum to weld itself to the edge.

    But there are chiploads that do not burnish that are much less than the recommended chiploads which are aimed at MRR. Given that all chips leave a scallop behind but smaller chips leave a smaller scallop, you want to run less chipload to get a better finish.

    The biggest issue is most cutters don't have a documented edge radius to go by. You have to pick a guestimate. 20% of recommended chipload as the absolute lower limit is a pretty good guestimate in my experience, but if you want to be on the safer side use a higher percentage.

    Cheers,

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  4. #84
    Join Date
    Dec 2004
    Posts
    783
    I cut this last night, using the 3 flute 1/8" viper endmill, 14000 rpm, 25-30 ipm .03" DOC.

    I guessed at the rpm and feedrate based on test cuts and adjusted rpm for a nice sound. Used a water based lube/coolant from think&tinker in spritzes.

    would be Interested on the math here to compare with destiny tools specs. Maybe put the thread back on track, or have 4 of you come up with different numbers and argue about it

  5. #85
    Join Date
    Oct 2011
    Posts
    0
    Quote Originally Posted by Dylwad View Post
    I cut this last night, using the 3 flute 1/8" viper endmill, 14000 rpm, 25-30 ipm .03" DOC.

    I guessed at the rpm and feedrate based on test cuts and adjusted rpm for a nice sound. Used a water based lube/coolant from think&tinker in spritzes.

    would be Interested on the math here to compare with destiny tools specs. Maybe put the thread back on track, or have 4 of you come up with different numbers and argue about it
    You would benefit from a much larger endmill. 1/4 or even 5/16

  6. #86
    Join Date
    Oct 2011
    Posts
    0
    Quote Originally Posted by UWP_Wes View Post
    So let me get this straight, the one flute end mill is designed for routers because they cannot run their spindles slow enough?

    The reason for the single flute end mill is that they cannot get the feed rate high enough to get the chip load where it needs to be to prevent the flutes from clogging. The way you describe it is just confusing.

    You need to be very careful about advising people to slow their feed rate in aluminum. Slow feed rates in aluminum lead to BUE and flute clogging. You have to maintain the chip load to prevent this.
    Lol dude.. don't even bother with Bob. I spent 7 pages arguing with him about this to the point he went whining to the moderators

  7. #87
    Join Date
    Feb 2006
    Posts
    7063
    Quote Originally Posted by Dylwad View Post
    I cut this last night, using the 3 flute 1/8" viper endmill, 14000 rpm, 25-30 ipm .03" DOC.

    I guessed at the rpm and feedrate based on test cuts and adjusted rpm for a nice sound. Used a water based lube/coolant from think&tinker in spritzes.

    would be Interested on the math here to compare with destiny tools specs. Maybe put the thread back on track, or have 4 of you come up with different numbers and argue about it
    Unless you're running on a very lightweight mill, you should be able to do roughing at a MUCH deeper DOC. I do most of my roughing with 1/8" tooling at a 0.100" DOC, and comparable RPM-adjusted feedrates (8200 RPM, 18 IPM), with HSS tooling.

    Regards,
    Ray L.

  8. #88
    Join Date
    Dec 2004
    Posts
    783
    Quote Originally Posted by SirDenisNayland View Post
    You would benefit from a much larger endmill. 1/4 or even 5/16
    Not enough room, some of the slots are only .22" wide, and not a fan of tool changes unless the tools have depth rings.

    And its a one-off piece. I used a 1/4" end mill to surface both sides of the 3/8 extruded piece though.

  9. #89
    Join Date
    Dec 2004
    Posts
    783
    Quote Originally Posted by HimyKabibble View Post
    Unless you're running on a very lightweight mill, you should be able to do roughing at a MUCH deeper DOC. I do most of my roughing with 1/8" tooling at a 0.100" DOC, and comparable RPM-adjusted feedrates (8200 RPM, 18 IPM), with HSS tooling.

    Regards,
    Ray L.
    Its a cncrouterparts based 24x48x7" router with a 2.2kw water cooled spindle. Its modified from their design to be more rigid, but nothing like a real mill with flood coolant and power under 8000rpm.

    Also plunging .1" in aluminum scares me as the cam I use 99% of the time wont let you ramp into the cut, and cut2d isnt as user friendly for the one-off design-as-you-go pieces

  10. #90
    Join Date
    Mar 2011
    Posts
    525
    It looks like you are milling 5 sides, then flipping the plate and surfacing to separate the individual parts.

    How do you keep the small parts from being grabbed and destroyed when you flip you plate over and surface the other side?


    Quote Originally Posted by twocik View Post
    I cut small pieces like this all the time and can tell you use the machines spindle. The larger the cut diameter, the better. I design most of my parts around my tool library. I spiral rough (carbide coarse 3FL) cut and finish with a ZRN carbide coated 2 - 3 FL EM. Here's a few to show







    Final




    I also design a lot of fixtures to hold the parts for 2nd, 3rd, 4th, etc.. mop. I use to cut these with a .125" cutter but wanted more speed, so I dropped one part to save 5 mins or so on each plate. Anyway hope this helps, let me know if you need anymore help










    .
    Kelly
    www.finescale360.com

  11. #91
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by HimyKabibble View Post
    I do most of my roughing with 1/8" tooling at a 0.100" DOC, and comparable RPM-adjusted feedrates (8200 RPM, 18 IPM), with HSS tooling.

    Regards,
    Ray L.
    Ray, I managed to break 3 endmills this week using 2 flute solid micrograin carbide at 5100rpm and 3 ipm at 3/16 doc... just too much doc? Didn't really seem to matter how slow I went.

  12. #92
    Join Date
    Dec 2004
    Posts
    783
    Quote Originally Posted by kregan View Post
    It looks like you are milling 5 sides, then flipping the plate and surfacing to separate the individual parts.

    How do you keep the small parts from being grabbed and destroyed when you flip you plate over and surface the other side?
    It looks like the parts get bolted to another plate from underneath, one of the pics shows the back side of the parts after the last operation and you can see the bolts.

  13. #93
    Join Date
    May 2005
    Posts
    2502
    Quote Originally Posted by Spinnetti View Post
    Ray, I managed to break 3 endmills this week using 2 flute solid micrograin carbide at 5100rpm and 3 ipm at 3/16 doc... just too much doc? Didn't really seem to matter how slow I went.
    What was your width of cut (stepover)?

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  14. #94
    Join Date
    Oct 2011
    Posts
    0
    Spinnetti:

    Are you running coolant? Your speeds and feeds, as well as the depth of cut seem pretty conservative to me.

    Bob asked about your radial depth of cut (the width of the cut) because even at greater than half the width of your tool you're only looking at a max of .0003" chipload per tooth. As bob explained in an earlier post, this may not be enough for the edge of the tool to actually get "under" the material.

    This leads to excessive rubbing, chip welding, and ultimately broken tooling. As your width of cut reduces beyond half the cutter diameter your chipload decreases exponentially.

    What you may be experiencing is the effect of going TOO slowly. If you have no coolant running or at the very least an air blast this will happen all too quickly. Personally I've never had much luck running aluminum without at minimum an air blast.

    Cheers

    Edit:
    Also, theoretcislly climbing may help with the situation as it allows the cutter to bite into what would be the thickest portion of the chip first. If its not able to bite in and cut it may just be displacing material. But I know you have rigidity issues so they likely outweigh this option

  15. #95
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by SirDenisNayland View Post
    Spinnetti:

    Are you running coolant? Your speeds and feeds, as well as the depth of cut seem pretty conservative to me.

    Bob asked about your radial depth of cut (the width of the cut) because even at greater than half the width of your tool you're only looking at a max of .0003" chipload per tooth. As bob explained in an earlier post, this may not be enough for the edge of the tool to actually get "under" the material.

    This leads to excessive rubbing, chip welding, and ultimately broken tooling. As your width of cut reduces beyond half the cutter diameter your chipload decreases exponentially.

    What you may be experiencing is the effect of going TOO slowly. If you have no coolant running or at the very least an air blast this will happen all too quickly. Personally I've never had much luck running aluminum without at minimum an air blast.

    Cheers

    Edit:
    Also, theoretcislly climbing may help with the situation as it allows the cutter to bite into what would be the thickest portion of the chip first. If its not able to bite in and cut it may just be displacing material. But I know you have rigidity issues so they likely outweigh this option

    Hmm. I'm using flood coolant, and doing climb cuts, at 50% and more radial depth - up to 100% ... maybe I need to speed up and see what happens. I'll try other workholding too.

  16. #96
    Join Date
    Feb 2006
    Posts
    7063
    Quote Originally Posted by Spinnetti View Post
    Hmm. I'm using flood coolant, and doing climb cuts, at 50% and more radial depth - up to 100% ... maybe I need to speed up and see what happens. I'll try other workholding too.
    Try starting at a very shallow DOC, and high feed, then gradually increase DOC until you run into trouble. With a 1/8" tool, you should easily be able to cut at least 1/16" deep, probably more. What is the flute length on the tool? You want to use the shortest flutes that will do the cut. A larger shank also helps. My 1/8" tools are mostly 1/4" or 3/8" shanks.

    Regards,
    Ray L.

  17. #97
    Join Date
    May 2005
    Posts
    2502
    As Denis says, chipload is down around 0.0003". Recommended is circa 0.0015. You're at that 20% of recommended number I suggest as the absolute lowest to risk before rubbing. If the cutter is at all dull, you probably are rubbing it.

    You would probably be fine just upping the feed to about twice what you're running. Use Ray's method to be conservative since you've already broken a few. Recommended feed from G-Wizard for this cut is 10.7 IPM, FWIW.

    For hobby mills, also look very closely at runout. I broke 4 1/8" endmills one day due to a bad ER collet. The collet was new and a name brand, but it was in a cheap ER chuck. I kept measuring the chuck taper and seeing it was true. It wasn't until I checked it against the cutter shank that I discovered how bad it was--0.0015".

    That was plenty to kill a few endmills since the runout is additive to the chipload. That's probably not your issue given how low chipload was, but I always bring it up as worth looking at.

    Cheers,

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  18. #98
    Join Date
    Dec 2003
    Posts
    673

    Red face

    Thanks guys... I'll up the feed and work into the radial DOC. I also figured out how I will fixture it that should work better and not take forever... stay tuned - I'll report back when my new endmills get here

  19. #99
    Join Date
    Jul 2007
    Posts
    1602
    Quote Originally Posted by Dylwad View Post
    Not enough room, some of the slots are only .22" wide, and not a fan of tool changes unless the tools have depth rings.
    Methinks you are ready to learn about tool tables: CNC Mill Machining Videos look for the "Tormach Tool Change" link about 1/3 of the way down the page.

    bob

  20. #100
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by rowbare View Post
    Methinks you are ready to learn about tool tables: CNC Mill Machining Videos look for the "Tormach Tool Change" link about 1/3 of the way down the page.

    bob
    He doesn't have a Tormach - its a router machine... drifted off scope a bit there from the original topic of tormach/finish.

Page 5 of 6 3456

Similar Threads

  1. Tips on a really nice side milled finish in aluminum
    By Kerry Harrison in forum Bridgeport / Hardinge Mills
    Replies: 5
    Last Post: 12-29-2009, 04:29 PM
  2. how to improve surface quality?
    By davidsutton in forum Uncategorised CAM Discussion
    Replies: 4
    Last Post: 07-15-2008, 01:27 PM
  3. Replies: 22
    Last Post: 06-30-2008, 05:42 PM
  4. Surface Finish
    By life3970 in forum Mini Lathe
    Replies: 2
    Last Post: 11-07-2007, 07:00 PM
  5. surface finish
    By fadalman in forum BobCad-Cam
    Replies: 2
    Last Post: 03-03-2007, 08:30 AM

Posting Permissions

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