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
Welcome to The Phlatforum PhlatPrinter III

SketchUcam 1.1 Chat

Discussion in 'SketchUcam DOWNLOAD' started by kram242, Sep 4, 2013.

Page 2 of 3
  1. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    I have failed to find a problem in either 8 or 2013. inside cut with tabs if I click the cut it removes all of it, if I click a tab it removes only the tab. for folds, centerlines and pockets, it removes the 'cut' but leaves the lines, that it what it is supposed to do.
    maybe you can tell me what sequence of creating and editing the lines causes a problem with deletes?
     
    swarfer, Sep 18, 2013
    #26
  2. 7up

    7up Moderator Staff Member

    Offline
    Messages:
    1,090
    Trophy Points:
    38
    Location:
    Kentucky
    It must have been a one-time fluke as I can't re-create the problem.
     
    7up, Sep 18, 2013
    #27
  3. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    Your talking about using the context menu "erase all phlat edges" right?
    I tried to get it to do it and I could not replicate it either.
     
    3DMON, Sep 18, 2013
    #28
  4. 7up

    7up Moderator Staff Member

    Offline
    Messages:
    1,090
    Trophy Points:
    38
    Location:
    Kentucky
    Right Shaun. Guess it was just a one time glitch.
     
    7up, Sep 18, 2013
    #29
  5. gravityisnotmyfriend

    gravityisnotmyfriend Member

    Offline
    Messages:
    32
    Trophy Points:
    8
    The new sketchucam is working great for me. I had a plane design as a .dxf that a friend of mine emailed to me. It had all these lightening pockets milled in - and I had no way to replicate them with the earlier program. With the new sketchucam? It was a breeze. Took quite awhile with the 1/8th inch bit, though!
    [​IMG]

    [​IMG]

    [​IMG]
     
    gravityisnotmyfriend, Oct 18, 2013
    #30
    swarfer likes this.
  6. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    I wonder how much weigh it saves. Did you, by chance, weigh it before and after?
     
    TigerPilot, Oct 19, 2013
    #31
  7. gravityisnotmyfriend

    gravityisnotmyfriend Member

    Offline
    Messages:
    32
    Trophy Points:
    8
    I didn't weigh it. I could weigh a full sheet, then weigh the sheet that is left over from cutting the pieces out. The difference should be the weight of the plane in full thickness. Then, I could weigh the actual plane to see what the difference is.

    Though, that wouldn't account for the kerf on the full depth cuts. I guess the only way to know for sure is to cut out another one without the milled pockets.
     
    gravityisnotmyfriend, Oct 19, 2013
    #32
  8. andyr

    andyr New Member

    Offline
    Messages:
    1
    Trophy Points:
    1
    I have just started to use SketchUcam to drive a ShapeOko mill - really loving it. Has anyone used SU to generate laser cut files? I don't (yet) have a laser and the cutting services I use want DXF. I found a gcode to DXF converter but it is very buggy. One way of getting a DXF cut file would be to drop the original paths after creating the inside and outside cut paths and then export to DXF - does this make sense?

    --
    Andy
     
    andyr, Jan 21, 2014
    #33
  9. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    Andy, I have no idea what you're talking about with the dropping of the original path and so on but I did once recover a lost .dxf file by using the g-code. I used one of the programs that convert g-code to .dxf. I do not recall which one it was. I do remember that it was a pain in the neck. Especially if the part is complex. The reason is that the part is bigger than the original, by the size of the radius of the the bit, on each side and has to be scaled down accordingly.
     
    TigerPilot, Jan 21, 2014
    #34
  10. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    You could drop (or phlatten I assume) and convert it to dxf and would probably be what you would need to do if you had to have a dxf.
     
    3DMON, Jan 21, 2014
    #35
  11. Greg H.

    Greg H. New Member

    Offline
    Messages:
    5
    Trophy Points:
    1
    This is an awesome plugin!
    Great job!

    Any future plans for tool change, v carving and multiple hole depth options?
     
    Greg H., Jan 29, 2014
    #36
  12. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Tool change, yes, a sort of a plan. for one of my ideas I need to know tool length, and knowing that lends itself to tool change, or at least selection, as part of the preamble code. Not too many DIY guys have a tool changer though so this is not a priority for many.

    V carving you can do right now, just figure out how deep you need it and tell the parameters that is how thick the material is, then use 100% cut depth. lines drawn and set as 100% deep centerline cuts will then Vcarve just fine.
    After setting up the cuts you will want to experiment with grouping them, this affects the cut sequence optimization when you are using multipass and can significantly improve speed.

    multiple hole depth options? what do you mean?
    it can already do holes of any % depth, and any size above bit diameter (spiral bored). read the help!
     
    swarfer, Jan 29, 2014
    #37
  13. Greg H.

    Greg H. New Member

    Offline
    Messages:
    5
    Trophy Points:
    1
    Thank you for the info! To be more specific on the hole depth thing. I am trying to make a counter sunk hole for a 5mm screw and am hung up on trying to get the depth set for the larger part to the smaller part of the hole!
     
    Greg H., Jan 29, 2014
    #38
  14. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    ah. you will need to make 2 drawings, one for the through holes, and another for the counter sinks, since you cannot place 2 'holes' on top of one another. in fact any line intersecting the little purple line in the 'hole cut' symbol will cause trouble with the Gcode generation. I like to mark hole centers with a little triangle, with the top right corner indicating the hole position. The triangle sides must be less than half bit diameter.

    I do the basic drawing and make sure I have a reference L of lines at bottom left where I will position the bottom left corner of the safe area box.
    Then I copy and paste the whole thing outside the current safe area.
    now on the first drawing I'd put in the through holes, using the correct bit size etc.
    on the second drawing I'd put the partial depth holes for the counter sunk parts.
    (yes you can set partial depth AND larger than bit size on a hole at the same time)

    Now move the safe area box to the first reference, set the correct tool parameters, generate the Gcode.
    move the safe area to the second drawing reference, set tool parameters, and generate Gcode.
    now on the machine you zero the first tool and run the first gcode file, change tools, reset Z zero (XY are already correct!) and run the second file.

    This works perfectly, over Christmas I ran a job with 4 seperate files and 2 different bits and everything lined up perfectly (I also turned the part over to machine both sides but that is a seperate issue).
     
    swarfer, Jan 29, 2014
    #39
  15. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    You didn't say what size bit you are using so here are two ways to make it. One with a bit of 5mm diameter and two, one with a smaller bit.

    1) Draw the counter-sink circle. With the 'center tool' mark the center of the circle. Make the whole a group. Use the plunge tool in SketchUcam to mark the through hole, OUTSIDE OF THE GROUP. Don't forget to set the percentage to 102%, or so, before marking the hole. Go into the group and select the pocket tool. Set the percentage to the depth you wish and make the pocket.

    2) Draw the counter-sink circle. With the 'center tool' mark the center of the circle. Make the whole a group. Outside the group make the spiral bore as swarfer mentioned and inside make the pocket as I wrote above.
     
    TigerPilot, Jan 29, 2014
    #40
    swarfer likes this.
  16. Greg H.

    Greg H. New Member

    Offline
    Messages:
    5
    Trophy Points:
    1
    Awesome that help me very much!
    Looking forward to more features!


    Thank you!
     
    Greg H., Jan 29, 2014
    #41
  17. Greg H.

    Greg H. New Member

    Offline
    Messages:
    5
    Trophy Points:
    1
    Cant find the spiral cut option on pocket tool! Just zigzag and boundry cut!
     
    Greg H., Jan 30, 2014
    #42
  18. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,578
    Trophy Points:
    48
    When you select the plunge tool, just before you click on the position that you want the hole, press shift and then click on the position. A box will open asking you for the diameter of the hole you want to drill.
     
    TigerPilot, Jan 30, 2014
    #43
    marcomartim likes this.
  19. Greg H.

    Greg H. New Member

    Offline
    Messages:
    5
    Trophy Points:
    1
    Got it I! Thank you!
     
    Greg H., Jan 30, 2014
    #44
  20. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Some new things to look for in 1.1c
    phlat-announce-2.png
    At the top, buttons for saving and loading tool profiles. read the help!
    These options also available on the Tools|Phlatboyz menu as below, for those that cannot see the webdialog
    parameters menu.

    phlat-announce-1.png
    Options Summary displays a dialog with your current settings from MyConstants.rb, just for reference (probably editable in next version).
    Display Profiles Folder opens a file explorer in your profiles folder, so you can easily add .tpr files to it, or extract them to give to others, via the forum at this link.
     
    swarfer, Feb 14, 2014
    #45
    kram242 likes this.
  21. scott geisler

    scott geisler New Member

    Offline
    Messages:
    8
    Trophy Points:
    1
    Im looking for a little help
    when I put in the material thickness say 0.25
    then make a part and send to g-code it makes all z axes 0.35 can any one help me fix this problem


    %
    (Generated by SketchUcam {1.1d})
    (Bit diameter: 1/8")
    (Feed rate: 8' 4"/min)
    (Material Thickness: 1/4")
    (Material length: 1' 10" X width: 3' 6")
    (Overhead Gantry: false)
    (Retract feed rate NOT limited to plunge feed rate)
    (Optimization is ON)
    (www.PhlatBoyz.com)
    G90 G20 G49
    M3 S15000
    G0 Z0.1250
    X10.8568 Y5.8459
    G1 Z-0.3500 F100
    Y11.9709
    X23.2943
    Y5.8459
    X10.8568
    G0 Z0.1250
    G0 X0 Y0 (home)
    M05
    M30
    %
     
    scott geisler, Apr 22, 2014
    #46
  22. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    Change your In/Outside Overcut % in the parameters.
     
    3DMON, Apr 22, 2014
    #47
    swarfer likes this.
  23. Adverse Effects

    Adverse Effects New Member

    Offline
    Messages:
    13
    Trophy Points:
    3
    why carnt i set tabs to more than 80%? some of the stuff i cut is 30mm thick and 80% makes the tabs 6mm and i almost need a small saw to cut them and then i have to dress them with a sander or file
     
    Adverse Effects, May 13, 2014
    #48
  24. marcomartim

    marcomartim Member

    Offline
    Messages:
    195
    Trophy Points:
    18
    Location:
    São Carlos - SP - Brasil
    This functionality is very cool; I am increasingly impressed with the development
    But, once activated, the setup dialog appears every time I go to use (is uncomfortable)
    Would have a way to disable when I just want to make more holes with the diameter of the cutter?

    Hugs.
     
    marcomartim, May 13, 2014
    #49
  25. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    I don't know why it was limited to 80%, there are no comments in the code to explain it.
    So, you can just edit it yourself, the beauty of open source ...
    open the file 'whereyoursketchupis/Plugins/PhlatScript.rb'
    and jump to lines 239, 240,241
    it looks like
    Code:
      
def PhlatScript.tabDepth=(tdepth)
    Sketchup.active_model.set_attribute(Dict_name, Dict_tab_depth_factor, [tdepth.to_i, 80].min)
  end
    change the '80' to '99' and save, restart sketchup.
    now you can go to 99% depth.
     
    swarfer, May 13, 2014
    #50
Page 2 of 3

Share This Page