Hole interpolation accuracy with endmill
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 74
  1. #1
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default Hole interpolation accuracy with endmill

    Listen, I am sure this has been covered a number of times in different threads, but I wanted to ask the question. We interpolated a 1.002" hole with a .5" diameter 2" loc garr endmill in aluminum. The machine is a 2007 daewoo 3016 with cat 40 taper and fanuc Oi-mb controller. We used a bore gauge to check the diameter of the hole. The hole size tolerance is -0 +.001. The machine had no problem holding that size, but the hole size variation from interpolation is about .00035 to .0004. I assume this could be from a number of things. Possible endmill/toolholder runout, endmill deflection since it is a 2" loc, and/or backlash. If this variation is all from backlash, is .00035-.0004 acceptable or should I try to get it closer?

    If I can account for the backlash in the controller, how do I do that? Or is it even needed if .00035 is close enough?

    Thanks,

    Chris

  2. #2
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default

    Oh and by the way, I am using all i,j, and k in the programming. I am not using R's.

    Chris

  3. #3
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,901
    Post Thanks / Like
    Likes (Given)
    514
    Likes (Received)
    896

    Default

    Sweep the hole with an indicator to confirm your roundness/lobing. A bore gage only checks opposite sides. Probably close but. . .

  4. #4
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    509

    Default

    Sooo many variables.

    What are you speeds/feeds? More importantly, what are your look ahead / shape comp settings?

    Sure, backlash can be comped out, but an out-of-round hole doesn't tell you anything about backlash. A lost motion check is really easy to do, and will tell you a lot more.

    Let's start by looking at your process, and then go from there.

  5. #5
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default

    we are using smoothing and feed optimization. We are using fusion 360. The tolerance set for smoothing is .00001

    Feeds and speeds: 2000 rpm, feedrate of 10 ipm. It is aluminum and we could have gone faster. The machine has an 8000rpm spindle so we try not to go too fast. This is a one-off part so we didn't apply super super fast feed rates for production.

    I do not know how to apply look ahead in fusion or on the machine. How do you do this?

  6. #6
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,741
    Post Thanks / Like
    Likes (Given)
    2255
    Likes (Received)
    1154

    Default

    If the entirety of the hole falls between the min and max, you're in.

  7. Likes reddman liked this post
  8. #7
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default

    The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

    Chris

  9. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    509

    Default

    Quote Originally Posted by cgrim3 View Post
    I do not know how to apply look ahead in fusion or on the machine. How do you do this?
    It varies by builder. I recommend that you investigate this. Fusion dumping out path at a resolution of .0001in won't mean anything if your controller is defaulting to .005in shape compensation.

    Typically on a Fanuc you are looking for G08 or G05.1 to turn on basic lookahead. Often the builder will also provide auxiliary codes for fine tuning.

  10. Likes Hardplates, Jeffery71 liked this post
  11. #9
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    509

    Default

    Quote Originally Posted by cgrim3 View Post
    I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane.
    I can easily comp an interpolated hole by .0001in increments on our DMG MORI, and can check with a deltronics pin accordingly.
    However, checking with a pin does not actually verify the form of the hole. I can guarantee that when I interpolate a hole to within .0001in diameter (and it passes a check with pins) that the hole is not round within .0001in. The pin check (and usually the customer) won't notice if it's a little oblong.

    Having a tight machine is critical, but a tight machine doesn't help anything unless your process control is actually good enough to achieve repeatable and measurable results.

    All that said - you can get a ballbar test done on the machine. That is basically the ultimate test of it's ability to travel in an accurate circle. Ballbar tests are often publicized for the best machines on the market. There are very few machines in the world that can interpolate a circle within .00001 to .00005, and that's before we even consider process variability.

  12. #10
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,911
    Post Thanks / Like
    Likes (Given)
    1056
    Likes (Received)
    1227

    Default

    A lot is going to depend on the control as well as the machine but often G05.1 Q1 is simple HPCC smooth interpolation mode (which turns short lines into arcs) and G5.1 P1 is multibuffer which is lookahead. Pretty sure this is FS15 format

    Moving at 10 IPM and having an actual arc as a toolpath I doubt you will see any difference with high speed codes

  13. #11
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,911
    Post Thanks / Like
    Likes (Given)
    1056
    Likes (Received)
    1227

    Default

    Quote Originally Posted by cgrim3 View Post
    The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

    Chris
    I highly doubt that, 0.0001-0.00005 yes

  14. #12
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,249
    Post Thanks / Like
    Likes (Given)
    326
    Likes (Received)
    782

    Default

    Throw it across a CMM and you start to learn that nothing is really round or cylindrical LOL.

    Something that I just need to hold a 0.001" tolerance zone? I would probably helical bore / interpolate for one-off or short run but I'd bore or ream for anything more than a handful of parts. I have found that the surface finish isn't as good helical boring but it seems to take up some of the slop by averaging it out as it goes around in a circle several times.

    Once you get to sub-thousandth for cylindricity call I'm going to be boring or reaming for sure.

    But I'm not exactly an experienced machinist so take that FWIW.

  15. Likes mr.greenman liked this post
  16. #13
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,741
    Post Thanks / Like
    Likes (Given)
    2255
    Likes (Received)
    1154

    Default

    Quote Originally Posted by cgrim3 View Post
    The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

    Chris
    "Threading the needle is a task for the young." I have a five year old machine that's only ever been used by me, for prototypes and short runs, and that gets a laser and ballbar calibration every year. On a 14 year old machine, yeah, especially if it's been run at or near capacity, I think you'd need a rebuild to get that accuracy back.

  17. #14
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default

    Do most of you guys do a laser and ball bar calibration yearly? How much does that usually cost you?

    Chris

  18. #15
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,499
    Post Thanks / Like
    Likes (Given)
    1637
    Likes (Received)
    2081

    Default

    Most* of the people boldly proclaiming very small numbers on interpolated bores don't have the experience or the measuring equipment to back it up.

    Pretty easy interpolate a hole on size with a tight tolerance just measuring the diameter with a bore mic, gauge, or pins. Most interpolated bores are not round, not cylindrical, not straight, but you need more sophisticated equipment or techniques to recognise such.

    Like Rick said, put your perfectly interpolated hole on a CMM or Talyrond and get a nice reality shock.

    People frequently recommend helical interpolation to get better holes, but that only addresses taper.

    There is no substitute for single point boring when you need holes that you can count on.

    FWIW, a good way to remove steps due to lost motion, or lobing from imperfect motion control, from an interpolated bore/boss or profile is to do an additional finish pass in the opposite direction. Climb mill first, then conventional. I guess doing this in combination with helical would be about the best you could ever hope to achieve by interpolation.

    *Obviously there are exceptions, no need to get mad if you're one of those who know what you're doing.

  19. Likes Hardplates, mr.greenman, Kyle Smith liked this post
  20. #16
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,741
    Post Thanks / Like
    Likes (Given)
    2255
    Likes (Received)
    1154

    Default

    The ratio of cutter size to hole size plays a part as well. Skim a 1" hole with a 1/8" endmill, and you'll see every imperfection of the machine's movement show up on the hole wall. Cut a 1/2" hole with a 3/8" endmill, and any errors will be minimized.

  21. #17
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,741
    Post Thanks / Like
    Likes (Given)
    2255
    Likes (Received)
    1154

    Default

    Quote Originally Posted by cgrim3 View Post
    Do most of you guys do a laser and ball bar calibration yearly? How much does that usually cost you?

    Chris
    About $1800 for a VF-3SS with a trunnion. It would be about $550 less without the trunnion. I use PQI here in MN.

  22. #18
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,911
    Post Thanks / Like
    Likes (Given)
    1056
    Likes (Received)
    1227

    Default

    Quote Originally Posted by gregormarwick View Post
    Most* of the people boldly proclaiming very small numbers on interpolated bores don't have the experience or the measuring equipment to back it up.
    I hope the equipment part is not true lol. A 50 millionth best test in the spindle will give you a damn good idea of roundness, well on a VMC anyway.

  23. Likes mhajicek, gregormarwick liked this post
  24. #19
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    42

    Default

    Damn 1800 bucks! That seems like a lot of money to spend on that every year

  25. #20
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,499
    Post Thanks / Like
    Likes (Given)
    1637
    Likes (Received)
    2081

    Default

    Quote Originally Posted by cgrim3 View Post
    Damn 1800 bucks! That seems like a lot of money to spend on that every year
    If you think that's bad, don't get a quote for laser mapping a gantry mill...

  26. Likes mhajicek liked this post

Tags for this Thread

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
  •