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

SketchUcam plasma cutting

Discussion in 'SketchUcam 'Most wanted Feature'' started by marcomartim, Apr 25, 2014.

  1. marcomartim

    marcomartim Member

    Offline
    Messages:
    195
    Trophy Points:
    18
    Location:
    São Carlos - SP - Brasil
    I think a good way to survival is the SketchUcam be used in other types of machines.
    Wish I could help it, but I lack technical knowledge.

    For use in cutting the plasma, it would be possible to implement the functionality to put SketchUcam start cutting off the tool path (with distinction between internal and external cut) with time to pierce the sheet and the ability to scale the distance and angle of entry for tool path?

    [​IMG]
     
    Last edited: Apr 25, 2014
  2. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    marco, I'll have to search it but I'm sure that there is a way to stop and restart the gcode if you want to change a cutting tool. I don't know if there is a timer function that will start it automatically but if there is, that's what you are looking for.
     
  3. marcomartim

    marcomartim Member

    Offline
    Messages:
    195
    Trophy Points:
    18
    Location:
    São Carlos - SP - Brasil
    Yoram;

    In plasma cutting, it is necessary to start cutting away part of the tool path at the beginning because the cut is necessary to drill the plate, the hole is irregular and deformed

    is also necessary to pause at the beginning of the cut motion in XY, for piercing the plate

    I manually edit Gcode in notepad to get the coordinates of the beginning and put G4 P. .. adicionat to the waiting time; but this is very laborious to do manually when there is many cuts to make.

    I have to trace the route SheetCam plasma cutting (I'm happy with it), but I believe the SketchUcam with sketchup would be a wonderful tool for this service

    example of gcode edited:

    %
    (Generated by SketchUcam {1.1d})
    (Bit diameter: 3,2mm)
    (Feed rate: 2000,0mm/min)
    (Plunge Feed rate: 1200,0mm/min)
    (Material Thickness: 1,0mm)
    (Material length: 3000,0mm X width: 2000,0mm)
    (Overhead Gantry: false)
    (Retract feed rate NOT limited to plunge feed rate)
    (Optimization is ON)
    (www.PhlatBoyz.com)
    (ECM defaults)
    G90 G21 G49 G61
    M3 S30000
    G0 Z10.000
    X30.665 Y16.205
    G1 Z-0.500 F1200
    G4 P3
    X37.728 Y21.284 F2000
    X28.450 Y28.404
    X21.331 Y37.682
    X16.855 Y48.487
    X15.328 Y60.082
    X16.855 Y71.677
    X21.331 Y82.482
    X28.450 Y91.760
    X37.728 Y98.880
    X48.533 Y103.355
    X60.128 Y104.882
    X71.724 Y103.355
    X82.528 Y98.880
    X91.807 Y91.760
    X98.926 Y82.482
    X103.402 Y71.677
    X104.928 Y60.082
    X103.402 Y48.487
    X98.926 Y37.682
    X91.807 Y28.404
    X82.528 Y21.284
    X71.724 Y16.808
    X60.128 Y15.282
    X48.533 Y16.808
    X37.763 Y21.270
    X37.728 Y12.584
    G0 Z10.000
    G0 X0 Y0 (home)
    M05
    M30
    %
     
  4. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Hi Marco
    I have plasma cutting on my list of things to do in Sketchucam.
    A great difficulty is that not all plasma machines operate the same way, yours has Z motion, but some do not, some need a 'torch on' code, others do not. This makes getting it working for everyone quite a problem, especially since I do not have a plasma cutter myself to experiment with.

    A similar difficulty is generating the lead-in and lead-out paths. Looking at your drawing you have an outside cut with extra lines. When I do that I get no Gcode generated (because outside cuts want to be closed faces), how do you do it? I can do it if I draw the cutline and set it as a centerline cut. Easy enough to draw in the lead-in/out lines like this, but automatic would be nice.

    When doing it automatically, where does one start? How long must it be?

    One thing I know for sure is that plasma code cannot be generated with optimization active as the optimization will prevent it starting at the end of the line if some middle segment is closer to the last cut point.

    I am also looking at generating code for a drag knife tool :)
     
  5. marcomartim

    marcomartim Member

    Offline
    Messages:
    195
    Trophy Points:
    18
    Location:
    São Carlos - SP - Brasil
    Good news you're thinking about it

    In most machines, the Gcode is similar.
    On machines whose THC controls the Z axis, any movement in the Z Gcode is ignored after an M command and some VB script (mach3)

    In many cases, the manufacturer of THC provides the plugin and the script needed to optimize the operation of the plasma cutting

    If you commit to develop a solution I assume the commitment to purchase a plasma generator and take the tests

    The extra line outside (or inside as applicable) are the most difficult, the program has to automatically generate this line (figure)

    [​IMG]

    Making the cut by a central line is a good solution when I need to make a cut, but when I need to cut several pieces, or pieces with many holes, is unfeasible edit any drawing to include lines outside (or inside)

    SheetCam in the beginning of the cut (S1, S2, _ Sn...) is set automatically (as in SketchUcam) but it is possible to change the location of the operator to optimize the cut
    (I quote SheetCam because the program is that I have)
     
    Last edited: Apr 26, 2014
  6. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    With all the extra care that has to be taken into consideration with plasma cutter it looks to me like it will need a separate module, like the phlat bone, only more complicated.:rofl:
     
    swarfer likes this.
  7. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    wow
    does it have to be an arc?
    if it is a straight line, what angle should it be at?
    if an arc, must it be tangent to the line segment?

    PS: the one thing you will not find on the web at this time is any kind of decent guide to generating Gcode for this sort of thing.

    right now I doubt we will ever have the ability to select the start of a cut in SketchUcam, the internal structure of sketchup makes it very hard to do this. this is why I programmed the cut optimization that finds the closest point on the new cut, to the last point on the old cut. in practise this is working very well for reducing G0 travel time. combined with the group reordering tool, I think we have a winner.

    What I might do instead is a modified optmization that finds the closest 'end' to the origin and always starts there, and generates the lead-in and out when it generates Gcode. they will never be visible in the drawing.

    anyhow, thanks for the input, I'm still thinking it through while working on some other things.
     
    kram242 likes this.
  8. marcomartim

    marcomartim Member

    Offline
    Messages:
    195
    Trophy Points:
    18
    Location:
    São Carlos - SP - Brasil
    No need to be arch, it is a refinement of Sheeetcam

    The angle should favor the movement, it is best to be tangent to the line drawing (or tool path), but it's not something critical, it may be 45 degrees

    would be ideal, but between good and very good , the best is what is possible
    Do not focus on the curved line, a straight line at 45 degrees this very good
    I put the bow, just as an illustration

    I understand your difficulty, but in the background it can not exist
    Gcodes to the router and plasma are very similar, the big difference for plasma cutting is to create the line off the tool path , the rest can be equal to (but refinements are welcome)

    The start location of the court as in routers is also not a clear serious problem that the closest to the ideal is best

    I appreciate your interest and effort
    With small steps, we can achieve a breakthrough.

    Hugs
     
    Last edited: Apr 26, 2014
  9. EpicenterBryan

    EpicenterBryan New Member

    Offline
    Messages:
    1
    Trophy Points:
    1
    Here is a new one for you to think about:

    The problem I am running into is that lots of GCODE generators including the PhlaytBoys plug in for Sketchup are outputting shortened versions without the leading root command once the first one is sent, unless it’s changed from the last one. Here is an example output from your plugin for Sketchup. This probably works fine with GRBL or Mach3 but not Marlin /Repetier-Host . Notice the change from G17 to G2 but then no more G2’s for ever until another command like G3 comes into play.


    G17 G2 X58.085 Y75.801 Z-8.820 R48.413
    X53.250 Y87.473 Z-8.820 R48.413
    X51.601 Y100.000 Z-8.820 R48.413

    Change it like this and its fine:

    G17
    G2 X58.085 Y75.801 Z-8.820 R48.413
    G2 X53.250 Y87.473 Z-8.820 R48.413
    G2 X51.601 Y100.000 Z-8.820 R48.413

    I have played enough with GRBL to know I hate the tools for transferring files, lack of LCD display and card reader support and the silly way to make changes to the firmware via a terminal command prompt. And I really don’t want to go back 2 decades and mess with that old Mach3 interface and PC’s with parallel ports, Lazycam and the rest of the old dog programs.

    I think one simple change to the plug in would be a button to “generate full GCODE” . That is, put the leading G or M commands or what ever in front of each line. It would work for all the existing GRBL (or even Mach3, EMC users) but sets up for a forward upgrade path for something modern like Marlin on a Mega board. There will be a day when the UNO goes away and GRBL is very specialized to compile and run using hardware and registers on the UNO only.

    This came up for me mainly because I’m building a system that will have several uses: Plasma system with water table, vinyl cutter and router as well as being a 2′x2′ 3D printer. A simple swap of the build plate and head, and the same machine takes on new functions. It’s no big deal to hack Marlin to add G codes like coolant and spindle which I have done before or redefine what “Fan” does based on an external input or something like that. But it’s over my head how to rewrite sections of Marlin to keep track of what the last valid G or M code was. You plug-in does that now. How about giving us the option to turn that off so you output the leading command for each line? You know it hasn't changed, but how about putting it in there anyway as a click-able option?
     
  10. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    That is in line with the Gcode language standard.
    It CAN be done, but SHOULD it be done?
    As I said before, shortened codes are part of the Gcode standard.
    Maybe Marlin is the one needing the update so that it becomes properly standards compliant?

    In the early days of Gcode the machines had very little memory and computational power, so leaving off repeated codes saved memory and processing time, not to mention shortened the length of a punched paper tape required for a program (-:
    Nice machine idea. Marlin should already contain supporting code for keeping track of modal commands so extending it to handle G1/G2/G3 should not be too complicated.
     
  11. monkeyalien

    monkeyalien New Member

    Offline
    Messages:
    1
    Trophy Points:
    1
    Any progress on SketchUCam for plasma cutters? I've modified several ruby script files to be better suited for producing Gcode for plasma cutting with torch height control, such as only having the torch on when it's on the cutting path and removing the movement of the Z-axis while cutting. I'd like to specify pierce delay and a safe spot for the blowout in Sketchup while eliminating things like spindle speed and material thickness.
     
  12. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    no, far too busy on other stuff.
     
  13. misil

    misil New Member

    Offline
    Messages:
    1
    Trophy Points:
    1
    Location:
    Czech
    hello, i have too plasma cutter and same problem. But solution is a very simply. We need only one simply function for adding one point before cutting next contour.

    My idea:
    I want cutt cyrcle. I select "inside cut tool" and click on cyrcle contour. Cyrcle is now marked for inside cutting. Now i click on new tool (anything as "Add point") and move cursor on "inside cut mark" in cyrcle. Is automatic marked start point of cutting (for better orientation) and in position where i now click is created point X. Coordinates of this X are added in gcode before cyrcle cutting contour. It is all.

    Ideal feature is, if i can add new X point before other.

    Plasma (or high power laser) now will start on X point and not corrupt material on contour.
    ------------------------
    is possible add this function, or is here any possibility for adding point in current version?

    (Sorry for my english, I hope you understand me :)
     
  14. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    That's a good idea misil! I'll have to try it out. :good:
     

Share This Page