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

2-axis hot wire path planning?

Discussion in 'SketchUcam 'Most wanted Feature'' started by Jesse_S, Jun 14, 2019.

  1. Jesse_S

    Jesse_S New Member

    Offline
    Messages:
    4
    Trophy Points:
    1
    Location:
    Louisiana
    Hopefully I'm not missing something that is already there. I'm looking for a way to use SketchUp with a 2-axis hot wire cutter. Best I can come up with is to use the laser cutter settings and manually create a small narrow part that takes the path I would like from the origin to the actual parts and back so that the movement between parts doesn't cut through them and the hot wire doesn't turn off in the middle of the foam. Is there a way to get the travel path to avoid the parts, similar to the settings in 3d printer slicers that will avoid going across the top of a print to keep from leaving lines and errant drops of filament? Also would be nice if it left the wire on until it finished all of the cuts.

    If I failed to search for my answer properly I apologize in advance.
     
  2. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    While this is possible is it a massive fiddle to get it to work since all the entry and exit lines are generated automatically and there is no way to control it without a lot of manual editing, I know because I have done it. I imported the outline of a wing and mounted a hot wire bow on my Z axis. Then I had to manually edit the entry and exit points and also search and replace so that XY moves became YZ moves.
    This was so much hassle that I wrote an entirely different piece of software for this job (-:
    You can use it here http://swarfer.co.za/rc/wire/index.php

    I do have a newer version under occasional development. The new one is written in Python so that it integrates with LinuxCNC though it can be used independently. If you want to try it I will send it to you.
     
  3. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,576
    Trophy Points:
    48
    swarfer, are you going to publish that program? I'm sure that there are lots of people interested in it.
     
  4. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
  5. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,576
    Trophy Points:
    48
  6. Jesse_S

    Jesse_S New Member

    Offline
    Messages:
    4
    Trophy Points:
    1
    Location:
    Louisiana
    Thank you for the reply. After considering what you said, and the fact that I don't use foam to make model airplanes (although I wish I did), I ended up building a light weight 3 axis machine and mounting a hot knife to it. The only challenge I have now is that while the knife is plunging I get more melting than under normal XY movement. I have been manually creating a "tail" close to the origin to try to get the the outside cut tool to start far enough away from the finished piece that it does not get misshapen by the extra heat during the plunge.

    If I want to do multiple objects, I either need to join them with thin segments and then sand off the "sprue" left between them, or I have to produce them all separately and join the g-code. None of these are dealbreakers, but if you have any suggestions for how I might streamline the process, that would be fantastic.

    As an aside, I love how nicely SketchUCAM does circles and arcs in g-code, I never thought I could get .05 mm accuracy from EPS.
     
  7. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Hi
    some ideas:

    1 - set the plunge rate much higher so the plunge takes much less time and so cannot melt back at all/as much.

    2 - use open shapes. this means you cannot use the outside/inside cut lines but it does let you create defined start points.
    the process is something like this:
    draw your shape
    add an outside cut
    select the white face between the outside cut and the shape and delete it.
    triple click the outsidecut line and phlatten it (this removes the 'outside cut' setting but not the line).
    add a lead in line, and a leadout line and split the shape at that point. The leadin and out can be separated by a gap of 0.002" but not less.
    now use the centerline tool to set this as a cut line.
    add a 1% deep plunge hole at the start of the lead-in line
    triple click the cut line, hold CTRL and click the hole, right click and 'create group'​

    the effect of the above is to force it to start at the leadin line. the hole is a group, and groups cut first, then the closest end of the closest cutline. if you have more than one hole and cutline then you have to group each hole+cutline pair to force the start points properly.

    one problem area may arise if you edit the shape before adding the outside cut. this can cause 'restarts' during the cut because some lines go backwards (according to Sketchup). The solution to this is a plugin 'BZ tools' which has a 'convert to polyline' function. This will make sure that all lines in a selection form a continuous sequence.
     
    kram242 likes this.
  8. Jesse_S

    Jesse_S New Member

    Offline
    Messages:
    4
    Trophy Points:
    1
    Location:
    Louisiana
    Brilliant! Those were the key bits of information that I needed. I had been adding a little sprue to my shapes, but consistently getting the cut to start on them when they weren't the closest thing to the origin was impossible. I use "Vertex Tools" after the cut line is generated to make it just how I want it, then add the little plunge line.

    Only thing I can't get to work right is the depth of the plunge, I've tried a few things but it keeps defaulting to full depth. I've just been manually editing the GCODE to save a little time on that extra plunge.
     
  9. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Yes, the plunge tool defaults to 100% after every click. I remember trying to change this behavior and having a lot of problems.
    So, just make habit of hitting 1 then ENTER before each hole placement.
     
  10. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    another way is to lay down a patch of holes all the same depth and then move them to where they are needed, and delete the extra ones.
     

Share This Page