Hole interpolation accuracy with endmill - Page 3
Close
Login to Your Account
Page 3 of 4 FirstFirst 1234 LastLast
Results 41 to 60 of 74
  1. #41
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    847
    Post Thanks / Like
    Likes (Given)
    192
    Likes (Received)
    972

    Default

    Quote Originally Posted by Hardplates View Post
    It's been a while but I seem to remember being able to select the edge of the solid with contour which is not what you want. You want to hide the solid and make the sketch itself visible and select that. Maybe it's changed since I last used it since the bastards were making changes every week when I used it.
    In many situations CAM packages interpret solid geometry selections as splines (depending on a host of issues including the originating CAD package kernel, any sort of hole edge distribution etc). Spline data is posted as a host of small line segments and will be controlled by chordal deviation tolerance, smoothing, and G187 type corner rounding in the control. By drawing non-projected lines and arcs, you can force the CAM system to use traditional code (G01, G02, and G03).

    I suppose a person could make the case that the control then takes those G02s and G03s and applies a similar micro-segmenting algorithm; however, in most cases those are far less noticeable in surface finish and processing speed at the machine.

    Point being, avoiding spline geometry in CAM pays dividends, especially running Haas type machines that have minimal look ahead. My understanding is the Japanese machine do far better digesting spline based CAM.


    Sent from my iPhone using Tapatalk

  2. Likes Hardplates liked this post
  3. #42
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,139
    Post Thanks / Like
    Likes (Given)
    569
    Likes (Received)
    8304

    Default

    CNC interpolated holes will never be "round" like a boring bar but who has a $50,000 gauge to check this?
    For so many fits they are close enough and so easy to adjust to make any size even if only four point contact.
    Becomes what is a "good" circle and then what is a good hole.
    If making holes in a engine block you may get really fussy. If making a press fit dowel hole not so much.
    Bob

  4. #43
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    260
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    69

    Default

    Quote Originally Posted by mhajicek View Post
    No contest indeed. I sometimes get a print and model at 5pm, and put the part on the engineer's desk by morning. I can throw an endmill in and get it done; I don't have a full set of boring bars for all length and diameter ranges. 99% of the time the hole will be a locating bore or a press fit for a pin, so if the gauge pins say it's good, it's good.
    Not to mention the huge cost of a single boring head.

  5. #44
    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 G00 Proto View Post
    In many situations CAM packages interpret solid geometry selections as splines (depending on a host of issues including the originating CAD package kernel, any sort of hole edge distribution etc). Spline data is posted as a host of small line segments and will be controlled by chordal deviation tolerance, smoothing, and G187 type corner rounding in the control. By drawing non-projected lines and arcs, you can force the CAM system to use traditional code (G01, G02, and G03).

    I suppose a person could make the case that the control then takes those G02s and G03s and applies a similar micro-segmenting algorithm; however, in most cases those are far less noticeable in surface finish and processing speed at the machine.

    Point being, avoiding spline geometry in CAM pays dividends, especially running Haas type machines that have minimal look ahead. My understanding is the Japanese machine do far better digesting spline based CAM.


    Sent from my iPhone using Tapatalk
    That's pretty much what I was trying to get at. I believe most solids and surfaces are NURBS where sketch's are actual straight lines and arcs

  6. Likes G00 Proto liked this post
  7. #45
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,738
    Post Thanks / Like
    Likes (Given)
    2245
    Likes (Received)
    1151

    Default

    Quote Originally Posted by CORONA VIRUS View Post
    Not to mention the huge cost of a single boring head.
    Good ones anyway. I have a couple cheapies I use once in a while.

  8. #46
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    123
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    70

    Default

    0.0004 variation in hole size would likely mean the machine is cutting as good as it was ever stated to, your cutter is not deviating more than 0.0002" from the commanded position (per side). Assuming they go by the somewhat standard 0.0004" accuracy 0.0002" repeatability claims for machine that size/type.

    If you feel you should be getting better results, there is one trick you can try. After interpolating one of your holes, have the program jog the machine around a good percent of the tables travel instead of just going to the next closest hole. On box way machines there is a tendency to "squeeze" out some of the way oil when you do a bunch of moves in one little area (i.e interpolation), increasing sticktion and perhaps causing some inconsistencies. Jogging the machine some distance between holes might redeposit a nice even film of way oil, possibly giving better results.

  9. Likes CORONA VIRUS liked this post
  10. #47
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,738
    Post Thanks / Like
    Likes (Given)
    2245
    Likes (Received)
    1151

    Default

    One trick to eek out a little more accuracy would be to alternate climb and conventional passes; that'll cover up axis reversal marks a bit.

  11. Likes CORONA VIRUS liked this post
  12. #48
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    I wanted to update everyone. It turns out that the people we bought the machine from were overcompensating the backlash. After setting the backlash comp to zero on all axes, I get about 50 millionths backlash in all axes. lol

  13. #49
    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
    I wanted to update everyone. It turns out that the people we bought the machine from were overcompensating the backlash. After setting the backlash comp to zero on all axes, I get about 50 millionths backlash in all axes. lol
    When buying a used machine many people will check backlash with an indicator, but few check the control backlash values against the factory parameters

  14. #50
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,139
    Post Thanks / Like
    Likes (Given)
    569
    Likes (Received)
    8304

    Default

    Backlash comp done with a indicator and simple step moves back and forth is almost always wrong and way overdone.
    Bob

  15. Likes Hardplates liked this post
  16. #51
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,738
    Post Thanks / Like
    Likes (Given)
    2245
    Likes (Received)
    1151

    Default

    Most indicators have some hysteresis, which will appear to be backlash.

  17. #52
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,139
    Post Thanks / Like
    Likes (Given)
    569
    Likes (Received)
    8304

    Default

    Even with LVDTS there is static and dynamic motion and how servo loop work.
    End position is not running at 1500 IPM.
    This a rabbit hole with no end. Control loop people love this math. Arc is analog yet the control is digital and time sliced.
    What goes on between each time slice that the control sees, what are the time contrasts both electrical and mechanically.... Its a wonder these things work at all.
    Bob

  18. Likes mhajicek liked this post
  19. #53
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    I did not write a program to check backlash. I just checked it with a 50 millionths indicator with the jog handle. I know the best way to do it is to write a program but I haven't had time to do that yet. I will do that this weekend.

    I just changed the normal backlash comp. There is a rapid backlash comp too. Should I change this as well?

  20. #54
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,554
    Post Thanks / Like
    Likes (Given)
    2798
    Likes (Received)
    4286

    Default

    Quote Originally Posted by cgrim3 View Post
    Coronavirus, I'm not entirely sure how to do that in fusion. I don't think fusion gives you that level of control but I might be wrong

    I think you'd have to change the post to get that result in the code. Once upon a time controls required that you output quadrants, so it can be done. I don't think it would be as simple in Fusion as drawing 4 arcs. Might be easier to just hand code it if it's all circles.
    FWIW the HSM Post forum could probably tell you how to do it overnight, even how to toggle it on and off.
    HSM Post Processor Forum - Autodesk Community

  21. #55
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    To address the concern about whether you should select geometry or a skecth in Fusion 360 for creating your toolpath, I posted this question over on the fusion 360 manufacturing forum. We will see if any of the autodesk people respond.

    Chris

  22. #56
    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
    To address the concern about whether you should select geometry or a skecth in Fusion 360 for creating your toolpath, I posted this question over on the fusion 360 manufacturing forum. We will see if any of the autodesk people respond.

    Chris
    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.

  23. #57
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    Give me a sec I'm going to try it. Do you guys use ijk's or R's?

  24. #58
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    I created two different programs for interpolating a 1.002" hole with a .5" endmill. One program I just selected the geometry of the hole and on the other program, I selected a sketch I created. The programs are identical. I am not saying they will always be identical though. All I did was just a quick and dirty experiment.

  25. #59
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    194
    Post Thanks / Like
    Likes (Given)
    113
    Likes (Received)
    38

    Default

    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?

  26. #60
    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
    I created two different programs for interpolating a 1.002" hole with a .5" endmill. One program I just selected the geometry of the hole and on the other program, I selected a sketch I created. The programs are identical. I am not saying they will always be identical though. All I did was just a quick and dirty experiment.
    If the geometry selection was outputting 1 arc then the sketch selection will do the same as there is no way the code can get any more simple. Where selecting sketches should help is when the geometry selection outputs linear moves or tons of small arcs.

    As far as arcs I run IJK. I don't know if they are more "accurate" but I remember hearing about bores not matching up well if your fourth decimal place was an odd number or something along those lines. Also I seem to remember R not being able to make a complete helix like IJK can. Anyway R has some limitation where IJKs only drawback is it's slightly more "complicated" to fingerCAM


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
  •