1. Hey guyz. Welcome to the All New Phlatforum!



    Sign Up and take a look around. There are so many awesome new features.

    The Phlatforum is a place we can all hang out and

    have fun sharing our RC adventures!

  2. Dismiss Notice

Speed of Z

Discussion in 'SketchUcam 'Most wanted Feature'' started by generalsocial, Oct 28, 2015.

  1. generalsocial

    generalsocial New Member

    Offline
    Messages:
    23
    Trophy Points:
    3
    I've been cutting a lot of small parts with many features these days. I put the z save travel high to keep the cutter away from fixtures and whatever's around the table.

    Here's the problem, if I use a slow plung rate it uses that slow rate when jogging above the material.

    Ideally it would use the plunge rate in the material (below zero Z) and the jogging speed above that.

    What's been happening is I watch the z axis go up and down for 2h on a job. If I make it faster then I'm plunging to fast into the material.

    I'm going to figure out how to edit the code later (perhaps with a search and replace or something)... but has this been looked at? Or is there a feature there already I missed?
     
  2. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    What controller are you using?

    What you are describing is not normal operation, the Gcode does not do that, ie, it uses G0 motion, which is 'rapid' (not jog) and will be the maximum your machine can do. I use SketchUcam Gcode on a rather rudimentary controller on a machine that can rapid at 6000mm/min and it definitely does that speed between cuts! I will give an example video below.

    All G01 moves specify a feed rate with the F word

    here is an example, I just drew a rectangle within a rectangle and applied an inside and outside cut and it begins like this.
    on each line I will add a comment to describe what it does
    G90 G21 G49 G17 ; setup modes to make sure we get what we want
    M3 S15000 ; spindle on at 15000 rpm
    G00 Z6.300 ; move Z to 6.3 above material
    G00 X24.620 Y11.986 ; rapid to this position, first corner of internal cut
    G01 Z-3.520 F762 ; plunge Z cut to this position at 762mm/min
    G01 Y28.786 F1016 ; cut to position at 1016mm/min
    G01 X31.420 ; cut to position at 1016mm/min
    ....

    After setting the cut feed rate F1016, it does not need to repeat that since feed speed is modal, it gets remembered till it gets changed.
    In any decent controller feed rate only applies to G01 type moves (and G2 G3 arcs of course), while the max rapid rate of the machine applies to G00 moves.

    I asked you in another thread what controller you are using but you never replied.

    the next few lines are

    G01 Y11.986 ; cut to here
    G01 X24.620 ; cut to here
    G00 Z6.300 ; rapid raise Z
    G00 X8.400 Y8.400 ; rapid to new start point
    G01 Z-3.520 F762 ; feed Z at plunge rate
    G01 X61.600 F1016 ; cut to here
    G01 Y51.600 ; cut to here
    ....

    This sequence changes when 'use reduced safe height' is true (the default) and you are drilling plunge holes.
    In this case Z will rapid down to 1/3 of the safe height and then only retract that far during the entire hole drilling sequence.
    This, and all other options, are described in the help, accessible via the big blue question mark in the toolbar.

    The other variation is when ramping is on.
    Now the same cuts start like this
    G90 G21 G49 G17
    M3 S15000
    G00 Z6.300 ; safe height
    G00 X24.620 Y11.986 ; start of cut
    G00 Z0.200 ; rapid to near surface
    G01 X24.620 Y28.786 Z-1.660 F762 ; start ramp, using plunge rate
    G01 X24.620 Y11.986 Z-3.520 ; finish ramp
    G01 Y28.786 F1016 ; cut to next point at feed rate
    G01 X31.420
    etc

    Now, ramping uses the plunge feed rate but it can be much higher (depending on material), if not the same as the normal feed rate, unless you have some plunge holes that need to use a slower plunge rate. In this case I would separate the plunge holes out into a separate drawing so I can generate the normal cuts with a high plunge rate, and generate the plungeholes with the slower rate, then join the files.

    Here is some Gcode running on a machine with 6000mm/min rapids, cutting at 2000mm/min, with ramping
     
  3. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    upon some reflection I think I may have interpreted what you said incorrectly :fugly:

    maybe you meant that the Z downfeed from the safeheight should be faster till it is near the surface, the same way the current ramping does it?
    if so, then what you want is code like this

    Code:
    %
    (Generated by SketchUcam V1.4-0d2e)
    (Bit diameter: 5.0mm)
    (Feed rate: 2000.0mm/min)
    (Plunge Feed rate: 1000.0mm/min)
    (Material Thickness: 5.0mm)
    G90 G21 G49 G61 G17
    M3 S30000
    G00 Z20.000                    ; safe height is 20mm
       X28.827 Y28.174
    G00 Z0.500                      ; rapid to 0.5mm off the surface
    G01 Z-5.000 F1000        ; cut down to Z depth
       Y39.274 F2000
       X43.127
       Y28.174
       X28.827
    G00 Z20.000
        X8.500 Y8.500
    G00 Z0.500
    G01 Z-5.000 F1000
        X61.500 F2000
        Y61.500
        X8.500
        Y8.500
    G00 Z20.000
    G00 X0 Y0 (home)
    M05
    M30
    %
    
    is that correct?
    if so, look for the new version of SketchUcam on 1 November.... it will do it.
     
  4. generalsocial

    generalsocial New Member

    Offline
    Messages:
    23
    Trophy Points:
    3
    Wow, thanks for all the info... just starting to read it.

    I'm using Mach3 and a Zylotex controller...
     
  5. generalsocial

    generalsocial New Member

    Offline
    Messages:
    23
    Trophy Points:
    3
    Jackpot! That's what I meant. I'm excited to hear this it will save me hours. :)

    But I'm going to read your other reply since I might learn something about gcode or something. :)
     
    swarfer likes this.
  6. generalsocial

    generalsocial New Member

    Offline
    Messages:
    23
    Trophy Points:
    3
    Your new plugin version address this perfectly. Wow, what a boost in speed! And I can have safe safe-heights. :)
     

Share This Page