First Time CnC, Contour 3 help needed! - Page 3
Close
Login to Your Account
Page 3 of 4 FirstFirst 1234 LastLast
Results 41 to 60 of 67
  1. #41
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,170
    Post Thanks / Like
    Likes (Given)
    215
    Likes (Received)
    1044

    Default

    I would lead in with G46 or G47 to a point on one of the straight sides of the triangle. The lead in radius would need to be small enough to avoid clashing the cutter with the opposite sides of the pocket.

    I would G41 G46 A_._ to the midpoint of one side, move CCW around the triangle at feed rate from vertex to vertex to vertex and back to the starting point, and then G40 G46 A_._. The contour is so simple, you don't need to mess with G91 and G90 to increment the depths; simply type the path again at a new depth if that's what you want. Run the contour once with a big enough cutter to knock out the middle of the pocket, and then run the small cutter to sharpen the corners. Consider running with a radius allowance and then a clean-up pass with no allowance. Consider going around twice with your final pass to account for cutter bending.

  2. Likes Colt45 liked this post
  3. #42
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    Thank you for your answer didnt think it that way
    Next time, i will give this a try

    Do i program x/y to middle of the pocket before the lead in and the g41 x/y coordinates to midpoint of one side? (first point of contour?)

    How the control defines which way to lead in/out?

  4. #43
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,170
    Post Thanks / Like
    Likes (Given)
    215
    Likes (Received)
    1044

    Default First Time CnC, Contour 3 help needed!

    Programming the tool to be at the middle prior to downfeed and G41 is safest. If you use M70 the tool will move to the start position automatically. The control determines the lead-in direction based on G41 vs G42. I would not use G42.


    Sent from my iPhone using Tapatalk
    Last edited by rklopp; 07-30-2019 at 04:55 PM.

  5. #44
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    How accurate the lead-in distance "A" from middle to start point needs to be or does the control manage small errors itself?

  6. #45
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,170
    Post Thanks / Like
    Likes (Given)
    215
    Likes (Received)
    1044

    Default

    There is no error. The control moves the cutter from wherever it happens to be, center or anywhere else, to the start point of the lead-in arc. The control figures out the location of the proper start point based on the given value of A and the target point on the contour. You don’t have to calculate A. Just make it not so big that the cutter clashes with the opposite side of the pocket.


    Sent from my iPhone using Tapatalk

  7. Likes Colt45 liked this post
  8. #46
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    Do someone know what software update version is neesded to get this work whats shown in picture?
    Atleast cant get it to work, gives error 81 if i remember correct.

    Is there a way to update this feature?


    img_20200302_214107.jpgimg_20200302_212720.jpg

  9. #47
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,513
    Post Thanks / Like
    Likes (Given)
    2069
    Likes (Received)
    2875

    Default

    Believe the software is carried on E-proms on the individual boards.
    Would need to change those e-proms for ones that were programmed with a set having a higher software level.
    Cheers Ross

  10. #48
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    I had at last some time to play with Fusion 360 and had my first program successfully loaded to my deckel. Now i had error 93 with some of the blocks and those blocks contains g2/3 with Z move... This isnt possible?

  11. #49
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,513
    Post Thanks / Like
    Likes (Given)
    2069
    Likes (Received)
    2875

    Default

    There are at least two versions or levels of Dialog4 controls.....(contour3 likewise i believe))
    First version lacked the power of the later configurations.
    The difference is physical and is easily confirmed.
    If you look inside your control you will see the K10 ribbon cable running across the top of the cards between slot 8 through 11.
    Early version has an empty slot at position 8 so the left end of the K10 is open/not connected.
    Also the next slot (9) has a fully populated board (NPP 55) .
    If this is how your control is fitted out then it will not do real 3-D contouring ....Just does not have that capability, This is not a software issue, but rather a hardware problem.

    The later setup, has the #8 slot filled with an NEP 52 board and the K10 jumper is connected at its end to that board.
    If you do an MDI of a circular move (G2/G3) you should be prompted for a Z value if that prompt is not shown when entering the data then you don't have the full 3-D contouring capability . (no helical milling)

    Looking at the screen shot of your software....you have an NPP 54 which if i am not mistaken goes with the early version (no helical) , further i don't see an NEP 52...
    So i would say that to run a curve with a depth move, you will have to do it with points.
    Cheers Ross

  12. #50
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    So i would need to get my fusion 360 post processor modified so that z moves are done in separate block?

  13. #51
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,513
    Post Thanks / Like
    Likes (Given)
    2069
    Likes (Received)
    2875

    Default

    No...What you need to do is get the post to treat curves as a series of point to point moves ((X,Y&Z) to emulate your circle and depth move, given that i am correct on the build level of your control.
    Your machine can do simultaneous three axis moves,just can't contour in three axis at the same time.
    Cheers Ross

  14. #52
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    Here is an example of the code, how it should be to work with deckel?

    %
    (&%10/000000)
    N1 M9
    N2 G0 Z100
    N3 G17 T5
    N4 S+1200 G4 F1.0
    N5 M9
    N6 G0 X10.402 Y-11.629
    N7 G0 Z37.45
    N8 G0 Z27.45
    N9 Z25.55 F1000.
    N10 X10.425 Y-11.646 Z25.368 F333.3
    N11 X10.491 Y-11.693 Z25.204
    N12 X10.597 Y-11.764 Z25.072
    N13 X10.736 Y-11.847 Z24.984
    N14 X10.896 Y-11.93 Z24.95
    N15 G3 X10.896 Y-11.93 Z24.325 I1.233 J2.569
    N16 G3 X10.896 Y-11.93 Z23.699 I1.233 J2.569
    N17 G3 X10.896 Y-11.93 Z23.074 I1.233 J2.569
    N18 G3 X10.896 Y-11.93 Z22.449 I1.233 J2.569
    N19 G3 X10.896 Y-11.93 Z21.823 I1.233 J2.569
    N20 G3 X10.896 Y-11.93 Z21.198 I1.233 J2.569
    N21 G3 X10.896 Y-11.93 Z20.573 I1.233 J2.569
    N22 G3 X14.144 Y-11.376 Z20.45 I1.233 J2.569
    N23 G3 X11.225 Y-8.457 I-1.46 J1.46
    N24 X10.242 Y-9.44 F180.

  15. #53
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    102
    Post Thanks / Like

    Default

    Go to HaasCnc and down load a Lathe or Mill operators Manual for free.They have Basic Programming.

    https://www.haascnc.com/content/dam/...ual---2019.pdf

  16. #54
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,513
    Post Thanks / Like
    Likes (Given)
    2069
    Likes (Received)
    2875

    Default

    I would need a drawing in order to run the geometry through my CAM and generate the points required for this to work as its written.
    Cheers Ross

  17. #55
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    749
    Post Thanks / Like
    Likes (Given)
    1025
    Likes (Received)
    172

    Default

    Dialog4 uses a slightly different syntax compared to what you wrote- try this format and see what happens (like what Ross wrote above)

    N15 G3 X10.896 Y-11.93 I1.233 J2.569 Z24.325

    One way to evaluate if your machine control can make helical moves is by writing a block of code on the console in mode 11.
    Start a new program, then write a test block:

    Type "G3" as the first command in the block and then let us know what prompts are displayed. If your machine can do helical, it will prompt for F, X, Y, I, J, and Z.

    Not sure why you have multiple M9- that is the code to turn off coolant.
    The Haas manual is probably not going to help you much with programming a Deckel with Dialog or Contour control.
    Last edited by Colt45; 04-12-2020 at 09:53 AM.

  18. #56
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    I try to check these today, i have coolant disabled from the CAM, but i also wonder why M9 is double. I am again very thankful for your input

  19. #57
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    28

    Default

    G2/3 with Z infeeds doesnt work, 3 axis simultaneous linear moves are possible. Kind of stupid since it has a canned cycle for threads etc. Or is possible to do helical moves with G9 code?

  20. #58
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,513
    Post Thanks / Like
    Likes (Given)
    2069
    Likes (Received)
    2875

    Default

    Believe the canned thread milling cycle will only do one revolution coupled to one depth move equal to the thread pitch. This means that you can only use a dedicated thread milling tool where the
    tool has multi teeth. (No single point thread milling) All threads then are cut in one pass, up to the length of the tool insert.
    Simultaneous 3-d moves are really only point to point moves...not contouring, and that is how you must run the CAM post in order to make that control work with a 3-D contour.

    Cheers Ross

  21. #59
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    749
    Post Thanks / Like
    Likes (Given)
    1025
    Likes (Received)
    172

    Default

    G9 can do helical if you have the right software/hardware version- you can test it out the same way as described in post #55 above to test G2/G3.
    Open a program on the console using MDI, start a new block and then enter "G9". Follow the prompts and see if you get a Z prompt at the end.

  22. #60
    Join Date
    Jul 2020
    Country
    MALTA
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    good afternoon
    I just purchased a deckel fp4a contour 4 and I'm having an issue setting the tool height.
    As I borrowed a deckel manuals as my original one are all in Italian.

    So I used this program
    N1 G0 X0.0 Y0.0 Z100.0
    N2 G17 T1
    N3 S+0
    N4 G0 X40.0 Y40.0 Z5.0
    N5 G75 F1500 S+0 G3 X40.0 X15 Y20.0 Y.4 F100 Z-5.1 Z-5.1 Z-.050
    N6 G0 Z100
    N7 G0 X0.0 Y0.0
    N8 M30


    I'm setting the workpiece as zero with the cutter
    On mode 10 I'm setting the tool height 0 RL 0 as well.

    When I'm running the program the z axis will start at +5mm
    And will end the program z-.05mm


    Any ideas how to solve this issue
    Thanks in advance


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
  •