Hole interpolation accuracy with endmill - Page 4
Close
Login to Your Account
Page 4 of 4 FirstFirst ... 234
Results 61 to 74 of 74
  1. #61
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    7,361
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3593

    Default

    Quote Originally Posted by CORONA VIRUS View Post
    Not to mention the huge cost of a single boring head.
    You guys never used deVlieg Microbore cartridges ? Not expensive at all. Accurate.

  2. #62
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    192
    Likes (Received)
    972

    Default

    Quote Originally Posted by Hardplates View Post
    Try selecting geometry and posting code, then select a sketch and post the code and compare.

    I just tried opening fusion to give it a try and it won't run unless I update it by downloading the latest version. So there is a better chance of hell freezing over than me trying it.
    I ran a combination of holes in Fusion 360:

    A 1" hole created by selecting the solid on a clean edge (no change in Z all the way around). This yielded clean code with IJ nomenclature.

    A sketch always yielded IJ code.

    A hole where the selection geometry is not clean (ie the top of the hole is altered in Z by a radius cut or a slight angle to the part), yields a dimensionally correct G-Code, but it is broken into thousands of small line segments. This is markedly affected by changing the cut tolerance.

    Interestingly(with my post), a helical bore from clean geometry puts out code in traditional IJ nomenclature with a Z moves for each quadrant of the circle. This is unaffected by changing the tolerance.

    These same rules apply to cutting on any edge. If you do a traditional contour on a part and change off the solid (and it is standard lines and arcs), it will output traditional G01, G02, G03. If you attempt to chain around the same part, but there is a Z change in the solid edge, it reverts to spine technology and you will output very large amounts of code and depending on the cut tolerance, start to exhibit faceting of the surface.

    These same rules apply to all the cam systems I have played with. I good rule of thumb is to CAM the part and keep an eye on how big the file is... a simple hole in Fusion is ~400bytes (depending on lead-in, # of passes, and safety lines of code). A hole based on spine geo is 1.6kb. Pretty easy to see why Haas machines with their limited processing power start to choke.

  3. Likes Hardplates, cgrim3 liked this post
  4. #63
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,173
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    8318

    Default

    Quote Originally Posted by cgrim3 View Post
    Does everyone here use i,j,k's or R's? I was always told to use i,j,k's because they are more accurate. What do you all think?
    The math inside the control tracking the rad is the same. Technically on different borders one or the other is more accurate as it is all integer encoder counts happening.
    I like Rs for ease of use and understanding or tweaking the code. If the start at an angle IJK is tad confusing and the whole jump through hoops thing.
    Then there are intentionally untangent rads... but that not common.

    Inside the control has to work in axis counts not nice clean decimal numbers. Metric screws/encoders as mostly used do not map correctly to the inch system.
    This a whole another accuracy vs programmed problem. It is not only a least increment in the control but the system and each axis resolution.
    A ways back and no choice as there was no R as no real "cnc brains" or CPUs involved.

    Both solve to the same and any control now can do it with ease and the same accuracy.
    So which is easier to code, read or modify?
    Bob

  5. Likes cgrim3 liked this post
  6. #64
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    204
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    42

    Default

    This is very helpful info.

    By the way, after taking out all the wrong backlash comp values in the machine (which was set by the people who owned it before us, I was mistaken, the machine is a 2004 daewoo 3016 vmc), the backlash in all axes measured about 50 millionths. You all think this is good ? Then I applied backlash comp for the 50 millionths on all three axes. I tried to measure the backlash again after compensation and the indicator read dead nut on x, y, and z.

    The values for backlash comp were integers that were calculated by taking the amount of measured backlash, multiplying it by 25.4, then multiplying that by 1000 and rounding to the nearest whole number.

  7. #65
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    204
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    42

    Default

    I wanted to provide my method of measuring the backlash in case anybody has any better suggestions on the details of the process. Here is what I do. If you think you have a better way, feel free to chime in.

    1. We currently have a kurt vice in the mill. Say I am measuring backlash in the Y. I zero out the 50 millionths indicator on the back jaw of the vice. After zeroing out my indicator, I write down my Y value from the mill and I write down my Z value from the mill.

    2. Then I back off in the Y so the indicator is not touching the vice and I raise the Z up to clear the vice jaw. Then I jog the machine towards the back of the vice.

    3. After this, I bring the indicator back the other way to the Y value I wrote down before. I then move the Z down to the Z value I wrote down earlier. The difference in the measurement in the indicator is the backlash.

    The reason why I went through the trouble to type all this up is because I notice some people just set an indicator up in their mill and just move it back and forth while touching a surface the entire time. Is this a better way to do it?

  8. #66
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    204
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    42

    Default

    Does anybody have an opinion on this?

  9. #67
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    721
    Post Thanks / Like
    Likes (Given)
    175
    Likes (Received)
    521

    Default

    I think getting a tech in for an afternoon would be worth it's weight in gold right about now. Geometry checks are easy with the right tools and process, and they do it all the time. If you promise not to talk too much, most will even let you sit over their shoulder and watch, and show you where and how to adjust the comps.

    Not trying to be condescending, it just seems you have gotten in way over your head on this. You need to get yourself confidently back to zero.

  10. #68
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    204
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    42

    Default

    No we do not need a tech. The backlash is adjusted for. The most amount of backlash in the machine without any comp is 50 millionths.

    There are different ways of checking for it (i.e. writing a program and running the program with an indicator, jogging back and forth with the indicator with the handle, doing the procedure I wrote above).


    If you want to get the gist of what I was saying, watch this video here (go to 2:55):

    CNC Machine Setup and Alignment Part 8: Backlash - YouTube

    Basically, there are a couple ways of checking it.

    1. Write a program to do it

    2. Jog indicator back and forth while the indicator is on the surface the whole time.

    3. Do it like the man in the video (this is how I set mine)

    Which way do you guys get better results doing?

  11. #69
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,173
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    8318

    Default

    Quote Originally Posted by cgrim3 View Post
    No we do not need a tech. The backlash is adjusted for. The most amount of backlash in the machine without any comp is 50 millionths.
    That is insane good. To the point of are you sure.
    Something smells fishy. Not to say impossible but this is holy crap good.
    Ballbar?
    The video good and bad on many points. This is the basic and small shop view.
    Now why does this sort of comp not make perfect parts or holes/cylinders?
    Lets do circle and you are the computer. Axis change and backlash known. Where to do change to the servo paths?
    90 is way too late but what is the next path? Called AI by some but just looking ahead,
    Bob

  12. Likes Hardplates liked this post
  13. #70
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    204
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    42

    Default

    I'll try to post a video tomorrow of the backlash if the mill is free. But yes that is right, my dad and I both checked it with a 50 millionths indicator. I agree it does sound fishy hahahahah. I was very surprised as well. The machine has extremely low hours

  14. #71
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,173
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    8318

    Default

    I can not help and you have it all nailed.
    Do not bother with a video.

  15. Likes boosted liked this post
  16. #72
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    192
    Likes (Received)
    972

    Default

    I’m not smart enough, nor to I have the appropriate equipment. There is way more than just backlash to making an accurate contoured part on a mill.

    Backlash
    Servo tuning between the X and Y
    Friction tuning for differences between the X Y

    It’s an entire dynamic system, especially as velocities go up.


    Sent from my iPhone using Tapatalk

  17. Likes mhajicek liked this post
  18. #73
    Join Date
    May 2018
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    182
    Post Thanks / Like
    Likes (Given)
    139
    Likes (Received)
    92

    Default

    Quote Originally Posted by cgrim3 View Post
    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
    Can you run this same program now and measure the results?

  19. #74
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    4,359
    Post Thanks / Like
    Likes (Given)
    305
    Likes (Received)
    184

    Default

    Quote Originally Posted by Hardplates View Post
    If it were me I would be happy with 3 tenths on that machine and bore anything that needs to be held tighter.

    Often it is more valuable to know what your machine can and can't do than to have a machine that can do almost anything.
    Quote Originally Posted by CarbideBob View Post
    The math inside the control tracking the rad is the same. Technically on different borders one or the other is more accurate as it is all integer encoder counts happening.
    I like Rs for ease of use and understanding or tweaking the code. If the start at an angle IJK is tad confusing and the whole jump through hoops thing.
    Then there are intentionally untangent rads... but that not common.

    Inside the control has to work in axis counts not nice clean decimal numbers. Metric screws/encoders as mostly used do not map correctly to the inch system.
    This a whole another accuracy vs programmed problem. It is not only a least increment in the control but the system and each axis resolution.
    A ways back and no choice as there was no R as no real "cnc brains" or CPUs involved.

    Both solve to the same and any control now can do it with ease and the same accuracy.
    So which is easier to code, read or modify?
    Bob
    *Usually*, a machine that interpolates repeatedly to roundness within 10 microns (0.0004") is good to go.
    That is from experience in the UK from multiple service engineers with various makes/models of machines.
    I set a max limit of 3 tenths (8 microns) for my machines when ballbarring (Renishaw).
    The best I had was 4 microns (1.5 tenths 0.00015") but the average machine was 6 microns (0.00023").
    6 was about the best I could repeatable get without going mad and chasing my tail.
    Renishaw setup was the 100mm bar (so a 200mm circle) and a feed rate of F1000 (40"/min).

    Bob - ref the IJK against using the R value... I was told a couple of times by different people (AE's and Fanuc) that IJK is the most accurate because R leads to approximation/rounding errors. Where IJK are absolute figures.
    I believe mold work usually uses IJK for this reason.
    And ref the "math" being the same - when using the High Speed/Look ahead options (G05.1 etc), it's worth remembering that the control does use different parameters (acc/dec at least) than in "standard" mode.

  20. Likes Hardplates, Mud 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
  •