First Time CnC, Contour 3 help needed! - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 45
  1. #21
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    G41/G42 is modal, it stays on until you turn it off with G40.
    G45, G46, and G47 determine how you are going to approach the part-- parallel (G45) in a semi circle (G46), quarter circle (G47).
    When you enter G41, you get a prompt and an "A"- the A tells the control how far away from the XY coordinates of the contour to begin the approach.
    You can skip the G45, G46, G47 by pressing the "enter" key when prompted. and the tool compensation will be active without making one of the described approach moves.

    Drawing or a sketch of what you are trying to do would be a big help for us to help you.

  2. #22
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    I write all like this example says, i get code 83. I change block 6 g0 to g1 i get error n6 73 ? Whats wrong ???


    img_20181216_153242.jpg

  3. #23
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    Are you entering this direct on the console or transferring a file from a computer to your Deckel?

    Getting a "73" error in this case, means there is some kind of programming or computing error for which there is not a code. Dialog will sometimes display "an" error code when something is wrong, though the code isn't always specific to, nor descriptive of what the problem is. Usually the Block Number attached to the code is the Block where the problem is, or 1-2 blocks after. In your case, I don't think you did anything wrong if you are entering on the keyboard of the machine.

    Based on previous few posts in this thread, its probably a good bet you have some conflicting software or computing hardware in your machine-need to get that sorted out.

  4. #24
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    I enter direct on the console. I did not make the program till the end because i had the error in mode 8, i made it to n9 or n10.
    Is it a must to do the program to g40 to get it work without errors?

  5. #25
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    Not sure but maybe. Its a good idea to enter the complete sample program, especially right now when you aren't sure if your software is correct.

  6. #26
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    13,392
    Post Thanks / Like
    Likes (Given)
    2143
    Likes (Received)
    3328

    Default

    Quote Originally Posted by rklopp View Post
    I have a post-processor for Fusion 360 that I tweaked for Dialog 4. It's based on one that you can download from Autodesk.
    The post you started with, what control was it for?

  7. #27
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    I finished the code in the example to g40, now everything works

    It gives the error 73 when i change g00 to g01 but theres no need for the change. It will still aproach the cut with programmed feedrate. It moves with g00 to a desired position and then approaches with desired feedrate.

  8. #28
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    I use my old newbie thread

    Im going to mill a tool with insert pockets for tcmt 11 inserts. I have been thinking, what is the best method when it turns out to be abit small and i need To make it little bigger?

    Play with tool offset and "fool" the control with the tool diameter?

    How do you masters open up some contour pockets/shapes?

  9. #29
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    There are a few ways you can do it.

    Not a master, but have found this to be a good method if you have the tool doing other operations and do not want the rest of the program altered by changing the tool compensation in the Tool Register (Mode 10)- any compensation made in the Tool Register will apply to the whole program.

    Write the pocket using a canned cycle (like G71, G72, G73, G74), there is a line in the cycle block (called the "Finishing Allowance") for each axis which allows you to apply compensation to the tool. That compensation is in addition to any compensation you have in the Tool Register, but only applies in that block and will not affect the rest of your program.

    If you are machining a triangle shaped pocket, then you have to write out the contour and use tool compensation in the Tool Register.

    There are some other ways to accomplish this, including using "D" tool compensation (I do not ever use them for the sake of simplicity), if all you are doing is maching the pocket, .making changes in the Register will be simplest and easiest.
    Last edited by Colt45; 07-19-2019 at 07:37 PM.

  10. #30
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    How does the G79 work? Does the control calculate on its own to clear out the excess material? (between contours/Islands in an pocket)

    What is the Allowances for length/radius in the Tool Register used for?

  11. #31
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    Quote Originally Posted by Harri89 View Post
    How does the G79 work? Does the control calculate on its own to clear out the excess material? (between contours/Islands in an pocket)
    What is the Allowances for length/radius in the Tool Register used for?
    Haven't used G79 much and can't comment on that.
    The Allowances for length/radius in the Tool Register apply compensation to the tool everywhere in the program.

  12. #32
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    Was today doing some machining... Or atleast i tried, not with good succes..

    How do you write the program with the contour compensation on and infeed increments? (Example, 4x -z 3mm the same contour) I didnt get it to work...

  13. #33
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    129

    Default

    Several diffferent ways to do it, including a "repeat" with incremental Z moves

    Post a drawing of what you are trying to make and the code you are using thus far and we can help you troubleshoot it.

  14. #34
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    7,942
    Post Thanks / Like
    Likes (Given)
    1765
    Likes (Received)
    2305

    Default

    If you need to do depth steps on a contour that you are programming, one solution is to call the first depth before the contour call but enact it after the machine moves to start the contour and
    enables cutter comp.(M70)
    Write the depth in incremental using a G91, then the depth needed. Make that depth a multiple of the number of steps you need to make....So for example if you are going to a depth of
    say 20mm in three steps, the total depth needed with for example a 4mm clearance plane, would be 24mm.
    Three steps means each step would be 8mm per pass....So your incremental depth would be 8.0mm.

    Call and run the profile using cutter comp. Assuming that the cutter ends at the start point, do a repeat call (L) and enter the program numbers for the depth move and your contour programming.

    Additionally you can run a finished cut on both the depth and contour by using the tool modifier. In mode 10 where you have your cutters listed, you can add tools that have the same number but followed by an "*"

    Example: T1 R5.0 L0.0
    T1#1 R4.9 L-.01

    If you call T1*1 after the contour and repeat the contour the machine will adjust and take .1mm off each side of the profile and go deeper by .1.....(by my example)
    It does this without needing to stop, spindle remains rotating at programmed speed...happens on the fly, but if memory serves you must cancel cutter comp before using that call.

    Could also write the depth move in a sub routine and call it after each cut around the profile...

    Then you could also use the parameter programming (mode 12) and assign the depth as a variable...and have the variable be increased with each complete cut around the contour.
    The parameter programming is quite powerful, allowing the machine movements to be modified using math and formula statements...much like the lines in an Excell spread sheet....

    Disclaimer:
    Any programming advice here should always be tested by graphics or air cutting when testing new concepts or approaches....There are details in this stuff that can cause real trouble if not called or written
    correctly.
    Personally, i do most of my programming these days using a CAM system and so my manual programming is a bit dull, and some of this stuff might not be exactly correct.

    Cheers Ross

  15. Likes Colt45 liked this post
  16. #35
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    If i do a macro/subroutine with g91 for the in feeds example, do i have to call g90 again in the main program to stop g91 From the macro/sub?

    Would it be best to run the contour in a macro and do the in feeds in main program?

    I tried the in feeds in a subroutine but it made always an error. The contour was the main program. I use also G79 code to clear out the triangle pocket. I dont know if that G79 messes up something here?

    G79 is still abit mystery to me, first it asks feed increments and axis directions for clearing out and then the starting point and cutting directions to clearing out the pocket.

    From where it calculates the starting point and whats the difference with the axis directions and cutting direction?
    I assume these need always to be opposite axis?


    Hope you understand my bad english

  17. #36
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    7,942
    Post Thanks / Like
    Likes (Given)
    1765
    Likes (Received)
    2305

    Default

    To answer , Both the G90 and G91 are "Modal" commands, which means that once called they remain in force till they are
    changed....
    So if running absolute (G90) and you call G91 to do the depth move, you must reestablish absolute moves (G90) once the depth move has been executed.

    As to your G79....Hard to give an accurate answer.
    Post a copy of the code you wrote to run this and a sketch of the desired contour with dimensions and an indication of the part orientation relative to the machine axis as well as the machine "home " point.


    Cheers Ross

  18. #37
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    I made an macro from the pocket and got it to work with in feeds g91 and called g90 after that inside the macro. I still first had the same problem till i Figured out to write my Z2 position before the g79 to the main program.

    Its stil weird that it machines the pocket to a weire contour, like the programmed points would be way off. It seems that if i write a radius alot smaller than the tool, it does it better.

    Looks like the control cant handle small pockets?


    Now i have a problem with the g42 pocket milling. It mills start and end point past the desired point. And does that as sharp point. It does the same with g79.

    Should these tool paths be written with the tool centerline without g42 compensation?

    img_20190728_150917.jpgimg_20190728_150902.jpgimg_20190728_150906.jpg

  19. #38
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    Heres my hand drawn sketches if anybody understands of them anything....
    The smaller ones measurements are from bottom of a tcmt 11 insert. The bigger one is for the pocket.
    1, 2, 3 are the order where i am running it.


    I drilled first the corners with 4mm ball ensmill to 10mm depth and from there with 4mm drillbit, i use 5mm carbide end mill with 24mm cutting length. Pocket needs to be 22.45mm deep + 3.175mm for insert. The insert pocket im thinking to machine with 7deg. 3 flute taper endmill, bottom dia is 2.5mm and largest is 10mm.

    img_20190728_182019.jpgimg_20190728_182136__01.jpg

  20. #39
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    4,915
    Post Thanks / Like
    Likes (Given)
    169
    Likes (Received)
    862

    Default

    I am too tired from a day of international travel to do this reply justice, but I have a couple comments.

    I don't think you need to use G79/M79. That's for pockets with islands. I don't see an island involved in making a triangular pocket for a carbide insert. I have never used G79.

    Why G42? Climb cutting using G41 works better 99.99% of the time. It could be that G42 is cutting on the wrong side of the line you expect, which is why it gets better when you tell the control an artificially-small cutter radius. I don't see any G45/46/47 A_._ with your G42 and G40 blocks. Those govern the lead-ins and and -outs. Does Contour 3 not use lead-ins? You should use them if you can.

    Can you provide a clearer sketch showing what is pocket, what is metal, and what is air? If the pocket is within triangle 1-2-3, then I would use G41 and cut in the order of 3-2-1. I am guessing you are making a lathe toolholder, in which case a G45 linear lead-in starting at point 3 should work fine. If the programmed cutter diameter will fit in the pocket at all, then G41/G42 should work, you should not need to program the centerline, and you should not be using G79/M79.

  21. Likes AlfaGTA liked this post
  22. #40
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    10

    Default

    You can skip the g45/46/47 lead in/out by pressing enter. The only lead in/out would be possible from inside the triangle, this pocket is inside a cylindrical piece of annealed 4140.

    And there is an 90 deg.(45deg/2) Countersink inside from the 0 point in the picture where is the tcmt 11 inserts cutting edge. The pocket needs to be machines 2 times, 180degrees to each other

    So there is metal in every side of the cut. How would the control calculate this lead in/out?

    I used the G79 to clean out the middle of the pocket, maybe its just better to program it with 2 different dimensions and forget the g79


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
  •