Question for you Deckel NC owners
Login to Your Account
Results 1 to 6 of 6
  1. #1
    Join Date
    Sep 2009
    Post Thanks / Like
    Likes (Given)
    Likes (Received)

    Default Question for you Deckel NC owners

    Hi All,

    For the deckel NC owners out there what CAD/CAM do you use and is there
    a good post for your machine?


  2. #2
    Join Date
    Feb 2001
    Redwood City, CA USA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    I use Autodesk's Fusion 360. There is a post for Dialog 4, but it is piss-poor, and took quite a bit of modification to make is useable. It is still not very good, because it is easy to choke the control with too many small moves. For example, adaptive clearing is practically useless. There is a "smoothing" setting that turns a collection of small G01 straight moves into single G02/G03 arc moves, but it is not very smart and mostly only seems to work on the finish pass around a contour.

    I get the most success by using Fusion to extract the G-code for a contour with smoothing turned on and using compensation in the control (as opposed to the computer running the CAM). Then, I edit the code and copy the code running from G41 through G40 into a separate subroutine. I set up the main routine mostly manually to call the subroutine with whatever tool I want with whatever stock-to-leave or wear offset I want.

    Even then, the subroutine requires tweaking. For example, Fusion makes the lead-in and lead-out arc moves part of the contour, rather than using the G45/G46/G47 and A addresses. I end up deleting the arc moves and adding G45, G46, or G47 and an A value manually. The G41 block from the CAM also has no G01/G00 commanding the A approach. If the contour does not have to be super-precise, I manually use G64 and G61 at the end of the block, which helps keep the cutter moving at the expense of some accuracy. If I use G60 and G61, the control can choke and pause cutter movement, which marks the part, may lead to chatter, rubbing the cutter, and work-hardening the part. Occasionally Fusion CAM will generate a small straight move that is too small and Dialog throws an error. I think there might be a Fusion setting to fix that problem, but I have not found it.

    Here is a part which direct CAM would have made a huge G-code file. These are cycloidal gear teeth profiled with a 1/8" endmill.

    cycloidal-1.jpg cycloidal-2.jpg

    Instead, I made the code very compact by pulling out the code for a single tooth space and then repeating it while rotating the machine's coordinate system 2° with each repetition using G55. The code for one tooth space is the code after %23*10 at the bottom. The code makes a rough and finish pass through each tooth space. Pretty sweet if I do say so myself.


    T1 R1.587 A0.05 L0 A0
    T1*1 R1.587 A0 L0 A0

    N4 M9
    N8 G0 Z100
    N12 G17 T1
    N16 S+5000
    N24 G0 X-80 Y200
    N28 G0 Z6
    N36 Z5 F76
    N40 Z-0.1 F76 M70
    N44 F160 M70
    N48 %*10
    N60 G0 Z6
    N70 T1*1
    N80 S+5000
    N90 G0 X-80 Y200
    N100 Z5 F76
    N368 Z-0.1 F76 M70
    N372 F160 M70
    N396 %*10
    N410 G0 Z6
    N420 G55 W-2 I0 J0
    N430 L22 N24 N420
    N440 G53
    N732 G0 Z100
    N736 T0
    N740 M30

    N92 G41 G45 A3.2 X-80.333 Y189.242 G1 G64 M61
    N100 G2 X-77.67 Y186.582 I-10.835 J-13.51
    N104 G2 X-77.181 Y185.932 I-9.542 J-7.677
    N108 G2 X-76.728 Y185.156 I-4.493 J-3.145
    N112 G3 X-74.452 Y184.274 I1.607 J0.769
    N116 G3 X-73.426 Y186.49 I-0.665 J1.653
    N120 G2 X-73.639 Y187.363 I5.203 J1.732
    N124 G2 X-73.74 Y188.17 I12.095 J1.919
    N128 G2 X-73.672 Y191.933 I17.247 J1.571
    N140 G40 G45 A 3.2


  3. #3
    Join Date
    May 2002
    South Central PA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    FWIW I found a Deckel Dialog code generator here - Smartcam MIlling Code Generators for Smartcam. I haven't tried it yet, I haven't gotten to loading my old version of smartcam or trying a new version yet. I fondly remember how good the control was over every piece of geometry in Smartcam and think it will be a good match for the Deckel.

  4. #4
    Join Date
    Oct 2012
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    I have tried many CAM systems over the years, for many (dialog 4,11 millplus and HH430) controls.The problem is that all new CAM packages are oriented to modern controls, so they tend to create huge programs that make older machines work slowly and jerky, besides taking too much memory space. The only users I know of that are satisfied with their cam packages have older (15+ years) versions.

  5. Likes Mud liked this post
  6. #5
    Join Date
    Dec 2002
    Benicia California USA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    I use SurfCam.
    Has a generic post for Dialog4, but in reality it really dud not work.
    Ended writing my own.
    Surfcam has a dialog box choice when you post the code to select either G17 or G18 (horizontal or vertical) Not sure other programs give this option.
    Post is in two sections to make the correct code for vertical or horizontal.....(the X moves get flipped)
    Not the most wizz bang program, but i have had it for some time and its what i use.
    Biggest issue on the Dialog controls with a CAM program is that the control really has little look ahead, and tries to complete every move even if small. Making sure your post uses a G64 (blending)
    helps reduce the start/stop.

    Of course having the optional DNC setup is a real plus here if you are going to do any 3-D profiling.

    Cheers Ross

  7. #6
    Join Date
    Feb 2004
    Napa, CA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    I've been using OneCNC, it does generate a bunch of very small moves. On the HH 410 (my FP3NC) or HH430, these don't create much of a problem as the control can be set to effectively smooth them, the lookahead is efficient, and memory isn't a problem. The most recent version of OneCNC though (XR8), has an option to use arcs instead of small linear moves for things like HSM paths. The result is a code reduction of about 2/3 for those operations.

    Like Ross, I have two posts, one for vertical and one for horizontal, the same program can be run either way by using the right post.

Tags for this Thread


Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts