Deckel FP2NC Dialog4 Helix
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 27
  1. #1
    Join Date
    Oct 2020
    Country
    GERMANY
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Question Deckel FP2NC Dialog4 Helix

    My FP2NC shortly pauses after each G2/3 with X,Y,Z as it was in G60-Mode, although it is in G64-Mode. Is that normal?
    G2/3 with X&Y only it runs smooth as expected.

  2. #2
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    My FP2NC D4 does smooth helixes (helices?) within G41...G60 M61 //// G40... I use G09 polar coordinates. My machine has the latest software update that was available, although I forget the number... 3.7 maybe? What is your feed rate? Can you post a code sample?

  3. #3
    Join Date
    Oct 2020
    Country
    GERMANY
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    N10 G53
    N12 G90
    N14 G64
    N16 M62
    N18 G17
    N20 M9 M5
    N22 T1
    N24 S+800 F80
    N26 G0 X-1.643 Y-5.461 Z5
    N28 G0 Z1.125
    N30 G1 Z-1.625 F80
    N32 G1 X-0.276 Y-4.001
    N34 G3 X-1.643 Y-3.461 I-1.367 J-1.46
    N36 G3 X-3.103 Y-4.095 I0 J-2
    N38 G3 X-3.22 Y-4.225 Z-1.681 I3.103 J-2.903
    N40 G3 X-3.331 Y-4.359 Z-1.736 I3.22 J-2.773
    N42 G3 X-3.436 Y-4.497 Z-1.791 I3.331 J-2.639
    N44 G3 X-3.534 Y-4.639 Z-1.844 I3.436 J-2.501
    N46 G3 X-3.627 Y-4.784 Z-1.897 I3.534 J-2.359
    N48 G3 X-3.714 Y-4.932 Z-1.949 I3.627 J-2.214
    N50 G3 X-3.794 Y-5.084 Z-1.999 I3.714 J-2.066
    N52 G3 X-3.869 Y-5.24 Z-2.048 I3.794 J-1.914
    N54 G3 X-3.892 Y-5.292 Z-2.064 I3.869 J-1.758
    N56 G3 X-3.956 Y-5.448 Z-2.108 I3.892 J-1.706
    N58 G3 X-4.014 Y-5.604 Z-2.15 I3.956 J-1.55
    N60 G3 X-4.066 Y-5.763 Z-2.19 I4.014 J-1.394

    The first two G3s (N34+N36) run smooth, the following do not.

  4. #4
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    I don't think your G64 and M62 are doing anything. They are meant to be used within G41 and G42 tool radius compensation. Here is code for a 10-turn internal thread helix with a 2.772-mm radius and 0.5 mm lead (M5.5x.5) using the horizontal spindle. The tool starts down in the hole and spirals out counterclockwise. The entire helix is coded at N190.
    ...
    N120 G18 T2
    N130 S+3150
    N140 G0 X0 Y3 Z0
    N150 Y2 F60
    N160 Y-11 F75 M70
    N170 F125 M70
    N180 G41 G46 A1 X2.772 Z0 G1 G60 M61
    N190 G9 G3 M71 W3600 G90 I0 K0 Y-6
    N200 G40 G46 A1
    ...

    I am not surprised the ancient control pauses because it cannot keep up with the number of steps in your code. Use G41/G40 and G9 G3 (G2 for external thread, assuming climb milling) and life will be much better.

  5. #5
    Join Date
    Oct 2016
    Country
    SWITZERLAND
    Posts
    104
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    56

    Default

    Probably stalling the old D4 control, as already mentioned.
    Even Dialog11 can be stalled, if you try hard enough (I know) ;-)
    Your G-code is some weird spiral, if I simulate it?

    Thread milling works very well for me on my D4 with Software V2.32, but I do it in a single line with polar coordinates.

  6. #6
    Join Date
    Oct 2020
    Country
    GERMANY
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Yes, it is to chamfer are 3D-Spline. But it is not the complete code, it's even longer.
    screenshot_20211024_123535.jpg

    But the the G64 does something. If I use G60 instead with a simpler geometry, it pauses after each line.

  7. #7
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    The thread title word "Helix" threw me off. Now I see what you are trying to do, and I don't think there is a way to avoid the pauses. I have run into the same issue trying to cut a similar saddle shape. You can minimize the pauses by using a CAM program, turning on "smoothing" (which fits arcs to the path), and putting a big tolerance on the fitting between the arcs and the actual tool path in the design.

    I can't tell you why G64 does anything outside of a G41/G40 compensated path. I don't think it's documented in the manual.

  8. #8
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,668
    Post Thanks / Like
    Likes (Given)
    2874
    Likes (Received)
    4401

    Default

    Quote Originally Posted by rklopp View Post

    I can't tell you why G64 does anything outside of a G41/G40 compensated path. I don't think it's documented in the manual.
    I asked about G64 and didn't get an answer here. It's not documented well in my manual either. It does work outside of G41. I found that the G40 turned G64 off, and I had to put G64 on the next line if I wanted it to continue to be effective. When cutting a series of small arcs or line segments, G64 made it smoother and prevented the stops at the end of each segment even when cutter comp was not active.

    Having said that, I don't see anything in the OPs code that would turn it off. Do you still see G64 on the monitor while it is pausing? If you switch to distance-to-go mode do you see zeros on the screen for all 3 axes at the pause? If you turn the speed override way down to give the control more time to process does it still pause?

  9. #9
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,878
    Post Thanks / Like
    Likes (Given)
    2346
    Likes (Received)
    3282

    Default

    I agree with John...
    Believe that the G64 does work on code even when not using G41-42.....
    My post for SurfCam always calls G64 and it never uses the control cutter comp,
    CAM calculates the cutter offset within the program...code produced runs smoother and with less herk-jerk if i have the G64 in force....At least that is my experience.
    Never had any issues with it cancelling as the CAM does not use G40....

    Cheers Ross

  10. Likes Mud liked this post
  11. #10
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    9,811
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4708

    Default

    Quote Originally Posted by artelogic View Post
    N26 G0 X-1.643 Y-5.461 Z5
    N28 G0 Z1.125
    N30 G1 Z-1.625 F80
    N32 G1 X-0.276 Y-4.001
    N34 G3 X-1.643 Y-3.461 I-1.367 J-1.46
    N36 G3 X-3.103 Y-4.095 I0 J-2
    N38 G3 X-3.22 Y-4.225 Z-1.681 I3.103 J-2.903
    G's are not modal on a Dialog control ?

  12. #11
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    G0, G1, G2 & G3 are not modal. G81 82, 83 is not, either.


    Sent from my iPhone using Tapatalk

  13. #12
    Join Date
    Oct 2020
    Country
    GERMANY
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Mud View Post
    I asked about G64 and didn't get an answer here. It's not documented well in my manual either. It does work outside of G41. I found that the G40 turned G64 off, and I had to put G64 on the next line if I wanted it to continue to be effective. When cutting a series of small arcs or line segments, G64 made it smoother and prevented the stops at the end of each segment even when cutter comp was not active.

    Having said that, I don't see anything in the OPs code that would turn it off. Do you still see G64 on the monitor while it is pausing? If you switch to distance-to-go mode do you see zeros on the screen for all 3 axes at the pause? If you turn the speed override way down to give the control more time to process does it still pause?
    Will check that tomorrow. But I assume, the answer to my question is "yes it's normal, because the CPU is to slow".

    And yes, Gs are not modal. Omitted G is interpreted as G01.

  14. #13
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    9,811
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4708

    Default

    Quote Originally Posted by rklopp View Post
    G0, G1, G2 & G3 are not modal. G81 82, 83 is not, either.
    Antediluvian ! Gotta hand it to the germs, if they can make it unnecessarily complex, they will ...

  15. #14
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,878
    Post Thanks / Like
    Likes (Given)
    2346
    Likes (Received)
    3282

    Default

    Well at least you don't have to load the exe. with paper tape....
    And G1 might easily be seen as "modal' in that any move not otherwise defined is understood to be a G1....
    Cheers Ross

  16. #15
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    Antediluvian ! Gotta hand it to the germs, if they can make it unnecessarily complex, they will ...
    I don't view it as more complex, just different. In the modal, case, things get complex real fast if you forget to turn off modes like G0 or G81. Dialog is 35-year-old CNC, too.

  17. #16
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,668
    Post Thanks / Like
    Likes (Given)
    2874
    Likes (Received)
    4401

    Default

    Quote Originally Posted by AlfaGTA View Post
    Well at least you don't have to load the exe. with paper tape....
    And G1 might easily be seen as "modal' in that any move not otherwise defined is understood to be a G1....
    Cheers Ross
    Quote Originally Posted by rklopp View Post
    I don't view it as more complex, just different. In the modal, case, things get complex real fast if you forget to turn off modes like G0 or G81. Dialog is 35-year-old CNC, too.
    Tell him it makes plenty of sense when programming at the console, which is what the control is optimized for.

  18. #17
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    9,811
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4708

    Default

    Quote Originally Posted by AlfaGTA View Post
    Well at least you don't have to load the exe. with paper tape ....
    I like having the paper tape ! That way if something happens the damn control isn't just dead forever ...

    (Mine were all on mylar, btw. Lasts until the end of time, and if necessary you could read it manually. Paper tape is great ! )

  19. #18
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,878
    Post Thanks / Like
    Likes (Given)
    2346
    Likes (Received)
    3282

    Default

    Yep, and makes a nice companion to the "Lear" 8-track ya got under yer dash.....

    By the way, the Dialog controls (1-4) don't loose the executive,even is the batteries go dead and you never have to load it...
    Entire operating system is on E-Proms....
    Control fires up instantaneously, having no boot up, she is ready to run as soon as you push the start button....
    Cheers Ross

  20. #19
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    9,811
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4708

    Default

    Quote Originally Posted by AlfaGTA View Post
    Entire operating system is on E-Proms....
    Ja, that's what I'm talking about. When those go out, like bubble memory or magneto-optical with a lifetime of 200 years or my core memory that never goes bad, you're screwed.

    Sorry, I wuz bit by a 7400 nand gate as a youth, will probably never get over it

  21. #20
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,380
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1220

    Default

    Except you can still buy the E-PROMS.


    Sent from my iPhone using Tapatalk


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
  •