Fanuc C axis milling questions
Close
Login to Your Account
Likes Likes:  0
Results 1 to 6 of 6
  1. #1
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    284
    Post Thanks / Like
    Likes (Given)
    228
    Likes (Received)
    90

    Default Fanuc C axis milling questions

    I'm using a KIA SKT21LMS with a Fanuc 0i-TB and I'm trying to solve a couple of remaining issues. I'm not sure if they are postprocessor issues, machine parameter issues, or something else.


    1. [EDIT: Using G12.1 polar interpolation, so everything is in IPM]
    When interpolating a circle or helix close to X0 (milling out a shallow pocket on the face of a part, for example), the C axis has to turn really fast, and I get alarms like "excess error". If I turn feed rate override down while it's close to center, I can turn it back up later because the degrees/second required for a given feed reduce as you get further from center.

    Is there a param I can use to limit the speed it tries to rotate at? I'd rather hit a hard upper limit than get an alarm every time.

    I know I can program around this, but it would be better if I can just punch milling toolpaths out of CAM and not worry about it.

    [Edit: It could be spindle belt slippage too, causing the encoder to get upset...maybe? I am pretty sure I fixed that and I don't hear the characteristic squeak.]



    2. C coordinate direction. My CAM software wants to give C+ and C- values to indicate the direction the chuck should turn, but my lathe seems to only be expecting positive values. If I give it the + and - I get many extra rotations and if I were running a part it would end poorly. If I change all of the -C moves to +C it works fine.

    Everything I read online though seems to indicate that the + and - values are the norm, so is there a parameter that someone could have changed at some point to determine how it handles this?

    It also seems to behave a little different in radial milling vs face milling with regard to this.

    Same thing, I can change my CAM post to match if I have to, but to me it does seem like a good idea to know exactly which way things are going to go and not just hope that the shortest path is the correct one. I dug in the fanuc param manual and searched but did not find anything.



    3. Live tool holders- I have VDI40 live tools, and the previous owner must have used them a LOT. They're pretty wobbly. Like .01" of radial slop on each. I tightened up the preload on a radial holder a little to make it acceptable for some loose tolerance hole drilling, but 2/3 of them are no good for radial loads anymore.

    Is there any black magic inside or should I be safe to take them apart, clean, replace bearings (with suitable high spec ones, though anything is an improvement right now), lube, and run? I'm tangentially familiar with the principles behind bearing types, grades, preload, spindle design, etc so if I take my time I think I can rebuild them.

    It has just occurred to me that the above is assuming they are some sort of ball or roller bearing. If they're plain bearings, I guess I'd have to turn new ones and fit them to the shaft? That would be odd, but I'll have a look-see in a bit or wait for someone here to chime in and concur with or disprove my assumptions.


    Thanks in advance! I might add more to this as I think of it tonight.

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,114
    Post Thanks / Like
    Likes (Given)
    1126
    Likes (Received)
    2259

    Default

    Problem number 1, if it's at X0 that would be zero Degrees per Minute. Or Infinite Degrees per Minute. What you are asking is, is there a parameter to change Math and Physics? No, there isn't. You have to program around the fact. Program in IPM until you get suitable diameter then change. Honestly unless you are doing Simultaneous Axis work, DPM isn't really needed.

    Number 2, if this statement is true; snip>"If I change all of the -C moves to +C it works fine." then it's post issue. Change it to output the code you need.

    Number 3, go for it.

    R

  3. #3
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    284
    Post Thanks / Like
    Likes (Given)
    228
    Likes (Received)
    90

    Default

    Quote Originally Posted by litlerob1 View Post
    Problem number 1, if it's at X0 that would be zero Degrees per Minute. Or Infinite Degrees per Minute. What you are asking is, is there a parameter to change Math and Physics? No, there isn't. You have to program around the fact. Program in IPM until you get suitable diameter then change. Honestly unless you are doing Simultaneous Axis work, DPM isn't really needed.
    Obviously at X0 that's true, but the particular scenario is doing a helical entry to a circular pocket, or plunging at center and then spiraling out. So let's say X values >0 but still small. Should there be something capping the rotation speed, maybe clamping C at it's max and scaling X to keep it synced?

    Here's what FeatureCAM punches out as-is for a plunge and then spiral. I'm going to play with it a bit more, and see if I can get the post to at least output only positive C values and then keep troubleshooting the rest of it (whether the fix is in CAM, the post, or the machine).
    I just want to stop hand coding as much as possible. Maybe I'll just get a flat bottom drill or a boring bar that can plunge these shallow bores. They're 5" diameter, but shallower than a drill point on any reasonable size drill.

    N3 ( MAIN SPINDLE, Z-AXIS ROTARY TOOL )
    ( ROUGH1 POCKET HOLE7 )
    G0 G18 G40 G55 G80 G98
    T0909
    M43
    G28 H0.
    M111
    G97 S5000 M13
    G0 Z2.625
    X0.334 C0. M8
    G12.1
    G1 X0. C0.167 F50.0
    Z1.675
    Z1.425 F12.5
    G3 X0. C0.167 I0. J-0.167 F25.0
    X-0.3699 C-0.0206 I-0.0085 J-0.1766
    X0.0393 C-0.2047 I0.1958 J0.0118
    X0.4528 C0.0043 I-0.0094 J0.2161
    X0.0425 C0.248 I-0.2379 J0.0079
    X-0.5023 C0.0844 I-0.033 J-0.2537
    X-0.1857 C-0.269 I0.2574 J-0.0968
    X0.5792 C-0.0981 I0.1063 J0.2756
    X0.227 C0.3079 I-0.2965 J0.1126
    X-0.5239 C0.2228 I-0.1276 J-0.3076
    X-0.4413 C-0.2898 I0.2634 J-0.2368
    X0.5834 C-0.2503 I0.2352 J0.2914
    X0.566 C0.2904 I-0.2925 J0.2657
    X-0.6034 C0.3012 I-0.2978 J-0.2878
    X-0.5873 C-0.3371 I0.3021 J-0.3154
    X0.6881 C-0.3166 I0.3083 J0.3379
    X0.7171 C0.3313 I-0.3442 J0.3318
    X-0.0321 C0.4997 I-0.3697 J-0.3214
    X0. C0.5 I0.016 J-0.4997
    G1 Z2.625 F50.0
    M9
    G13.1
    M40
    M15
    G28 U0.
    G30 W0.

  4. #4
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,114
    Post Thanks / Like
    Likes (Given)
    1126
    Likes (Received)
    2259

    Default

    You have G98 specified. So don't worry about it. You have no G50 specified, but you have G97 specified.

    Have you tried variations of these?

  5. #5
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,536
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1389

    Default

    Quote Originally Posted by npolanosky View Post
    1. [EDIT: Using G12.1 polar interpolation, so everything is in IPM]
    When interpolating a circle or helix close to X0 (milling out a shallow pocket on the face of a part, for example), the C axis has to turn really fast, and I get alarms like "excess error". If I turn feed rate override down while it's close to center, I can turn it back up later because the degrees/second required for a given feed reduce as you get further from center.

    Is there a param I can use to limit the speed it tries to rotate at? I'd rather hit a hard upper limit than get an alarm every time.
    Hello npolanosky,
    If you were to draw a number of ever decreasing diameter, concentric circles and draw a chord of equal length on all circles, the angular distance between the two points of intersection of each chord with its respective circle becomes larger as the circle diameter decreases. Lets say that the length of each chord is 20mm and represented a Linear Interpolation and is the distance the tool moves per time unit at the feed-rate specified. As the Interpolation is a function of X and C movement, C must move at a greater rate as X gets closer to centre of the work-piece.

    If the feed-rate of the C axis exceed the maximum cutting feed-rate specified for the C–axis set in parameter (No. 1422), then an alarm will be raised.

    There is no parameter to work around this, but you can calculate the fastest feed rate that can be specified by F using the following algorithm (mm example).

    F = L × R × (pi/180)

    Where:

    F = mm/min

    R = Distance (in mm) between the tool center and work-piece center when the tool center is the nearest to the work-piece center.

    L = Maximum cutting feed-rate (deg/min) of the C axis.

    Obviously, by rearranging the above algorithm, you can solve for R, given a specified F, so as to obtain the diameter when the C axis Feed Rate will be exceeded and therefore, know at what point the Feed Rate in the program will have to be altered.

    If you can't get your Post to do that, it would be relatively easy to right a software routine to scan the program and add the appropriate Feed Rate where required.

    Regards,

    Bill

  6. #6
    Join Date
    May 2006
    Location
    Burlington, North Carolina
    Posts
    344
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    130

    Default

    Quote Originally Posted by npolanosky View Post
    I'm using a KIA SKT21LMS with a Fanuc 0i-TB and I'm trying to solve a couple of remaining issues. I'm not sure if they are postprocessor issues, machine parameter issues, or something else.


    1. [EDIT: Using G12.1 polar interpolation, so everything is in IPM]
    When interpolating a circle or helix close to X0 (milling out a shallow pocket on the face of a part, for example), the C axis has to turn really fast, and I get alarms like "excess error".

    Is there a param I can use to limit the speed it tries to rotate at? I'd rather hit a hard upper limit than get an alarm every time.
    We have several NT machines with 18i controllers so I don't know if it corresponds to your 0iTB or not, but I've found parameter 5450 bit 1 (AFC) to be useful. A quick look in your parameter book should tell you.


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
  •