G41 on a Speedio - mostly working
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default G41 on a Speedio - mostly working

    Trying to insert a G41 into code to tweak a bore size on a part. For some reason, if the call is before the G100 toolchange it doesn't work. The G40 is shown to be active while boring. If I do two consecutive bores and put the G41 in between, it works. My post processor (using Inventor HSM 2016, can't upgrade to current post, I tried) puts the G41 pass through before the tool change even though it appears to be after, see pic.

    Anyway, can anyone tell me what is cancelling the G41?

    Thanks

    G00 Z27.855
    G83 X45.108 Y-38.288 Z-24.616 R26.855 Q10 F1900
    X107.508 Y-38.266
    G80
    G00 Z37.855
    G41
    M05

    (BORE1)
    G54
    M09
    G100 T28 X44.766 Y-37.164 G43 Z37.855 H28 D28 S7000 M03
    M08
    G00 X44.766 Y-37.164
    G00 Z37.855
    G00 Z23.855
    G01 Z22.49 F1500
    G01 X44.76 Y-37.159 Z22.391

    g41.jpg

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,417
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    1688

    Default

    I could be wrong, but I think G41 has to be immediately followed by a G1. That G1 is where the offset happens. I could be wrong.

    Regards.

    Mike

  3. Likes CosmosK, Bobw liked this post
  4. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    My workaround is to cut air and put the G41 call in between. So this works:

    (cutting air)
    G01 X47.175 Y-37.273 Z24.034
    G01 X47.15 Y-37.229 Z24.105
    G01 X47.131 Y-37.198 Z24.184
    G01 X47.12 Y-37.178 Z24.268
    G01 X47.116 Y-37.171 Z24.355
    G00 Z37.855
    G41

    (BORE1)
    G00 X44.766 Y-37.164
    G00 Z37.855
    G00 Z23.855
    G01 Z22.49 F1500
    G01 X44.76 Y-37.159 Z22.391
    G01 X44.742 Y-37.144 Z22.294

    Your explanation makes sense. I'm just trying to understand. I was chasing this around for a good while.

  5. #4
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,980
    Post Thanks / Like
    Likes (Given)
    794
    Likes (Received)
    2424

    Default

    The G100 tool change will cancel the G41/G42.

  6. Likes CosmosK liked this post
  7. #5
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    cutting air it is, thanks for the help

  8. #6
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,005
    Post Thanks / Like
    Likes (Given)
    707
    Likes (Received)
    388

    Default

    I always thought you had to make an X and/or Y G01 move on the same line as G41 (and G40 for that matter.) I also thought you shouldn’t (or couldn’t?) make Z moves with cutter comp on. Apparently not!

  9. #7
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    951
    Post Thanks / Like
    Likes (Given)
    206
    Likes (Received)
    599

    Default

    Yeah G100 works as basically an "all the safety code" line so it kinda calls G80, G49, G40, etc.

    And just like FANUC you need a linear interpolation move between the G41/G42 call and the cut. HSM/Fusion 360 likes to use G18/G19 for the vertical lead-in radii but if you replace that with a linear move after the offset call it works fine in my experience.

  10. #8
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    965
    Post Thanks / Like
    Likes (Given)
    71
    Likes (Received)
    425

    Default

    I am not a brothers programmer but I have hand coded for 35+ years ... it looks like Brothers used a G100 for the tool call, and you would need a G41 or G42 "AFTER" the tool call in that it well reset the control to a G40 as soon as you called the G100 line ... Also there should be no GO0 ( rapid ) movers between your G41/G42 line and your G40 line ,, you cant rapid "any" axis well under cutter comp .

    Also your first G1 move after G41/G42 needs to be larger than your tool rad and the G40 move coming out of cutter comp needs to be longer than the rad

  11. #9
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    965
    Post Thanks / Like
    Likes (Given)
    71
    Likes (Received)
    425

    Default

    Quote Originally Posted by Rick Finsta View Post
    Yeah G100 works as basically an "all the safety code" line so it kinda calls G80, G49, G40, etc.

    And just like FANUC you need a linear interpolation move between the G41/G42 call and the cut. HSM/Fusion 360 likes to use G18/G19 for the vertical lead-in radii but if you replace that with a linear move after the offset call it works fine in my experience.
    no the G41/G42 call can be your first cut ,, it just needs to be longer than the rad of the tools

  12. #10
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    839
    Post Thanks / Like
    Likes (Given)
    1073
    Likes (Received)
    552

    Default

    Quote Originally Posted by D.D.Machine View Post
    I am not a brothers programmer but I have hand coded for 35+ years ... it looks like Brothers used a G100 for the tool call, and you would need a G41 or G42 "AFTER" the tool call in that it well reset the control to a G40 as soon as you called the G100 line ... Also there should be no GO0 ( rapid ) movers between your G41/G42 line and your G40 line ,, you cant rapid "any" axis well under cutter comp .

    Also your first G1 move after G41/G42 needs to be larger than your tool rad and the G40 move coming out of cutter comp needs to be longer than the rad
    Pretty sure the bolded part above isn't correct. That should even work on your Haas. IIRC I've used cutter comp on multiple profiles, with rapid Z up and rapid XY then Z down at new location. (I'm on the home confuser right now, and don't have code to pull and post from a program. If my memory is wrong, you have my apologies))
    I've often cut air when activating the comp, as noted above. Also Z up at the end, and cut air while turning compensation off.
    Agree that the linear move activating the compensation needs to be longer than the amount of compensation. (I think that what you mean above, even though you said rad)

    ETA: I just checked, and I can rapid with the cutter comp still active. I program with the post set up to automatically compensate for the nominal cutter diameter, and only compensate enough to tweak dimensions as needed. The move that activates the compensation needs to be greater than the amount of compensation - some people say "radius" - but that might be more than needed, just trying to be accurate in description.

    CosmosK - I'm not familiar enough with your CAD package to help with the post, sorry. Sure seems weird that the G41 is so far into the code, looking at post 18. I'm using the infamous BobCad-Cam. You might reach out to BrotherFrank. I've had wonderful support from Yamazen for stuff like this. I know he's really busy at this time, but I've found his advice to be excellent. Good luck!
    Last edited by eaglemike; 01-24-2020 at 12:39 PM.

  13. #11
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    951
    Post Thanks / Like
    Likes (Given)
    206
    Likes (Received)
    599

    Default

    Quote Originally Posted by D.D.Machine View Post
    no the G41/G42 call can be your first cut ,, it just needs to be longer than the rad of the tools
    That's what I'm trying to say - it functions exactly like FANUC where you need a linear move that allows the compensation to physically happen as you enter the cut. I can't recall if the C00 has a parameter that allows the G43 calls to be "virtual" instead of actual but I don't think so, I think the G43 also needs enough space to call and cancel during an actual move.

    I'd have to post some code out to check but I don't recall having to cancel and re-call radius compensation for positioning (G00) moves?

    Too bad the OP can't get the newest HSM post installed for whatever reason - the Autodesk Brother Speedio post is VERY squared away.

  14. #12
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    Quote Originally Posted by Nerdlinger View Post
    I always thought you had to make an X and/or Y G01 move on the same line as G41 (and G40 for that matter.) I also thought you shouldn’t (or couldn’t?) make Z moves with cutter comp on. Apparently not!
    The manual also indicates you need to call the tool # (G41 D#), but you don’t. In fact, I’m not sure I need to insert the G40 to turn it off… just let the next tool change do it.

    I got lots or errors when putting comp 0.5mm or more trying to test it out. I assume it would error out if the path didn’t like it.

    Rapids seemed fine.

  15. #13
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    Quote Originally Posted by Rick Finsta View Post
    Too bad the OP can't get the newest HSM post installed for whatever reason - the Autodesk Brother Speedio post is VERY squared away.
    Because I live in a cave. Perpetual license.. no maintenance, no updates, and I like it

  16. #14
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,082
    Post Thanks / Like
    Likes (Given)
    4634
    Likes (Received)
    3064

    Default

    What size hole and what size end mill are you using? I'll post it for my Brother and compare the two.

  17. #15
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    There are various sizes. One for example is 11.5mm with a 6.35mm end mill.

  18. #16
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    242
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    116

    Default

    Pretty sure you can get the cps file in the InventorHSM support forum, or just modify the one you have.

  19. #17
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    Not sure what to change. The pass through puts it at the end of the last toolpath. I don't know how I would get it to go between the TC and the paths associated with it


    Writes the specified optional block.
    */
    function writeOptionalBlock() {
    if (properties.showSequenceNumbers) {
    var words = formatWords(arguments);
    if (words) {
    writeWords("/", "N" + sequenceNumber, words);
    sequenceNumber += properties.sequenceNumberIncrement;
    }
    } else {
    writeWords("/", arguments);
    }
    }

    function onPassThrough( text ) {
    var lines = String( text ).split( ";" );

    for ( var i in lines ) {
    writeln( lines[ i ] );
    }
    }

    function formatComment(text) {
    return "(" + filterText(String(text).toUpperCase(), permittedCommentChars).replace(/[\(\)]/g, "") + ")";
    }

    /**
    Output a comment.
    */
    function writeComment(text) {
    writeln(formatComment(text));
    }

  20. #18
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    527
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    142

    Default

    Ok, I think I'm doing it wrong. I don't need to be inserting this as a pass through at all. there is an option in the tool path setup for "wear" compensation and it puts it after the TC and after the rapids:


    G100 T28 X44.575 Y-37.003 G43 Z37.855 H28 D28 S7000 M03
    M08
    G17
    G00 X44.575 Y-37.003
    G00 Z37.855
    G00 Z23.855
    G01 Z22.49 F1500
    G01 X44.569 Y-36.998 Z22.391
    G01 X44.552 Y-36.983 Z22.294
    G01 X44.523 Y-36.958 Z22.202
    G01 X44.483 Y-36.924 Z22.117
    G01 X44.434 Y-36.882 Z22.041
    G01 X44.376 Y-36.833 Z21.976
    G01 X44.311 Y-36.778 Z21.924
    G01 X44.241 Y-36.719 Z21.886
    G01 X44.167 Y-36.656 Z21.863
    G01 X44.091 Y-36.592 Z21.855
    G01 G41 X43.849 Y-36.386 D28
    G03 X42.954 Y-36.459 I-0.411 J-0.484

  21. #19
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,082
    Post Thanks / Like
    Likes (Given)
    4634
    Likes (Received)
    3064

    Default

    Quote Originally Posted by CosmosK View Post
    There are various sizes. One for example is 11.5mm with a 6.35mm end mill.
    Here is what my Mastercam post spits out for my Brother:

    (in inches)

    Doing 1 pass, starting from the center of the hole.

    (JAN. 24 2020)
    (1:21 PM)
    (MATERIAL - 1018)
    ( T1 | 1/4 FINISHER )
    ( CIRCLE MILL-- )
    N1 G100 T1 G00 G90 G54 X0. Y0. S3750 M03
    N2 G43 H1 Z2. M08
    N3 Z.25
    N4 G01 Z-.5 F75.
    N5 G41 D1 X.0148 Y-.0358 F20.
    N6 G03 X.1014 Y0. I.0359 J.0358
    N7 I-.1014 J0.
    N8 X.1013 Y.0045 I-.1014 J0.
    N9 X.0132 Y.0365 I-.0507 J-.0023
    N10 G01 G40 X0. Y0.
    N11 G00 Z.25
    N12 Z2.
    N13 G91 G28 Z0. M09
    N14 M30

    Starting at center, 45 deg line, arc into the hole, go around 1 time, arc off, 45deg back to center.
    hole.jpg

  22. Likes Bobw, CosmosK liked this post
  23. #20
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,211
    Post Thanks / Like
    Likes (Given)
    14799
    Likes (Received)
    11014

    Default

    This is exactly how its supposed to look.

    Courtesy of Mtndew.
    N4 G01 Z-.5 F75.
    N5 G41 D1 X.0148 Y-.0358 F20.
    N6 G03 X.1014 Y0. I.0359 J.0358
    I think what is needed here is to go back to basics.

    I think the basics of how cutter comp works isn't
    completely understood. Which is fine, it can be
    really confusing, I still fight with it on occasion,
    and I fought with it A LOT when I was first starting
    out.

    You mention "Wear"..

    Again. Back to basics. 2 kinds of cutter comp, and you don't
    want to mix them up, or BAD things happen (guess how I know that?).

    "Wear" is where you are programming to centerline. Your tool table
    is generally going to have zero's in it for D's. Then if you need
    to comp something, its only a few thou.

    The other type of comp. I'm not even sure what to call it. Full
    Radius Comp? Full Diameter? Should be in the same drop down box
    as you found "Wear" in. May be called "Machine", as in the machine
    does all the math.

    This is where the program coordinates are the actual coordinates
    of the part. The actual tool diameter (or radius) will be in
    your tool table. Lead ins and lead outs are a lot trickier than
    with "wear" comp.


    Pick ONE method and stick with it.


    Some people like running full r/d comp. I don't. I like "wear" comp.

    Why?

    Because I run a lot of stuff with no compensation at all. If I don't need
    it, I don't use it. I don't have to worry about what is in the 'D' register
    of the tool table, one less thing I have to worry about. I find it easier to
    program that way also, I'm not always messing with my lead in's and lead out's
    if I don't absolutely have to.

    Also double check how your machine is set up. Usually a parameter, but some use
    tool RADIUS, others use DIAMETER. Again, pick ONE and stick with it.

    Then comes the whole lead in and lead out thing, and trying to understand how
    that works.. But I've typed enough for now, somebody else can handle that.


    Once you wrap your head around it, its not too bad. If you had somebody
    sitting there with you, instead of trying to learn through a message board,
    it would have been a lot quicker also. The written word just doesn't
    come across as it should sometimes.

  24. Likes eaglemike 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
  •