Welcome to Our Community

Unlock hidden features. Sign Up for Free Today!

SketchUcam

Discussion in 'CAM' started by Mark Carew, Aug 13, 2015.

  1. Giarc

    Giarc Master
    Builder

    Joined:
    Jan 24, 2015
    Messages:
    493
    Likes Received:
    234
    Thanks!

    I am an idiot. :duh: I had only been clicking the links in the main body of the help page (holes in grid, etc...). somehow I had missed the menu at the top right.

    On the plus side, I tried using the table as z-zero. I like it. It guarantees I don't cut into the table. The foam I am cutting is not perfectly flat, so this seems to be a better solution.
     
    David the swarfer likes this.
  2. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Sketchup 2017 has been released.

    Yes, SketchUcam works in Sketchup 2017.
     
  3. mike wachowski

    Builder

    Joined:
    Nov 20, 2016
    Messages:
    1
    Likes Received:
    0
    i have same problem
     
  4. Kyo

    Kyo Master
    Staff Member Resident Builder Builder

    Joined:
    Feb 27, 2014
    Messages:
    574
    Likes Received:
    487
    Well worth joining the Phlatforum Forum. A lot of cool projects; not to mention the sketchUcam download .. :thumbsup:
     
    #34 Kyo, Nov 20, 2016
    Last edited: Nov 20, 2016
    David the swarfer likes this.
  5. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    I thought I had linked the github release here, but it must have been somewhere else. wow, major brain fart, sorry people.

    Anyhow, the SketchUcam resource now contains a link to the Github release.

    Please Please Please click the big blue question mark in the SketchUcam toolbar and then the 'what to do after install' link and follow the instructions.

    @samerhay80
     
  6. bnbellis3377

    bnbellis3377 Well-Known
    Builder

    Joined:
    Apr 12, 2016
    Messages:
    23
    Likes Received:
    6
    Hi
    I did the new update for SketchUp a few things are different now I'm wondering if sketchucam will work with the 2017 SketchUp?????
     
  7. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    880
    Likes Received:
    172
    Yes it will/does! :thumbsup:
     
    Mark Carew likes this.
  8. Gary Caruso

    Gary Caruso Veteran
    Builder

    Joined:
    May 19, 2016
    Messages:
    96
    Likes Received:
    53
    Been playing with some larger projects, like many counter bore holes for hold down inserts, and an engraved hex pattern for the vacuum table.
    Any good tutorials on cleaning up all the unnecessary Z lifts and rapids all over the place? I tried grouping the holes into rows and then selecting them with the order tool and that helped but it's not quick or super effective. The pic below is just a Hex grid with centerline cut 10% as an example.
    Thanks


    upload_2017-3-31_11-39-26.png
     
  9. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Sketchup does the weirdest things with group ordering on holes....
    Since the holes are created as groups to avoid interference from underlying geometry, it is group ordering that matters.

    Since you do have underlying lines I would do this....

    drawing 1:
    1. create the lines,
    2. create a marker for the 0,0 point for the safe area
    3. move safe area to the marker
    4. apply centerline cut
    5. generate Gcode to 'file1.nc'
    drawing 2: (can be just a new area in the same file, see my videos for details)
    1. draw a hexagon
    2. create marker for the 0,0 point THE SAME offset as done for the lines
    3. move safe area to the marker
    4. create markers that mark the centers of the bottom left most holes in the hex pattern. A small triangle that is left and down from the hole center works well.
    5. delete the hexagon
    6. now use the 'pattern of holes' tool to lay out a rectangular grid of holes for each of the hex corners. see drawing below.
    7. select all the holes, right click, Explode
    8. generate Gcode to file2.nc
    now use the joiner to join the 2 files.

    you can leave the holes grouped, and so long as you edit nothing after creating the holes, the holes will drill in the order they were created. However, in my testing I found that letting it optimize the order of the holes is nearly twice as fast, so explode them.

    for the grids, the dimensions you need are like this.
    hex1.png

    then you need corner markers like this: the top right corner is the mark for the hole center.
    you only need to set hole grids for the lower 4 marked holes.
    hex2.png
    then use the plunge tool, hold CTRL or ALT and click and enter the parameters for the grid:
    upload_2017-4-1_12-29-35.png

    and repeat for each of the lower 4 holes.
     
  10. Gary Caruso

    Gary Caruso Veteran
    Builder

    Joined:
    May 19, 2016
    Messages:
    96
    Likes Received:
    53
    WOW David you are the best! I still have a lot to learn when it comes to doing multiple layer files.
    Last night I already did the holes, I pulled the hex pattern off the drawing and moved it to another drawing.
    I'll run the drawings again and post the preview I get trying some of your tips. I'll have to do 3 or 4 hole patterns, what I did was use the move/copy and made a complete starter row then just repeated the move/copy vertically.
    Here is all the info...
    I have three drawings for this;
    First are the holes for the table, they are 6.3mm with a 10mm counter-bore and a 3/16" (bit dia) plunge on the hex corners. This took about 90min, travel all over the place
    IMG_3309.JPG

    Second is the actual Spoil board (1/2" MDF) has just holes but the holes that are over the threaded inserts are 1/4" and the holes over the plunge holes are 3/16. Took about 36min not to bad even with going all over the place.
    IMG_3310.JPG

    Third, the final step is the hex pattern but I had a hiccup, for some reason the pattern didn't line up with the holes even though I checked and double checked that I didn't mess up the drawing or the 0,0. Only thing I didn't try looking back (it is now the morning for me) is power cycle the Arduino, I did restart UGS which should be resetting the Arduino. I tried this twice with the same result even with re-generated G-code files (double-checking the geometry). It's not loosing steps or a loose pulley, and it comes back to perfect 0,0. When I re-ran it she went over the same lines.. lucky it's just a spoil board and the lines are not final depth, also still need to surface cut the board. :)
    IMG_3313.JPG
     
    #40 Gary Caruso, Apr 1, 2017
    Last edited: Apr 1, 2017
  11. Gary Caruso

    Gary Caruso Veteran
    Builder

    Joined:
    May 19, 2016
    Messages:
    96
    Likes Received:
    53
    Much Better, I made the holes again using the pattern (alt key) feature and it was no different in terms of crazy travel pattern, then I exploded the holes. :) Here is the result befor and after exploding...

    before AHHHH!!
    upload_2017-4-1_12-1-58.png

    After Exploding all the hole groups! :D
    upload_2017-4-1_11-59-59.png
     
  12. Gary Caruso

    Gary Caruso Veteran
    Builder

    Joined:
    May 19, 2016
    Messages:
    96
    Likes Received:
    53
    Got the HEX pattern lined up, still don't know why it was off last night but this morning i re-ran the g-code and it worked great.
    Thanks for your help David, I think the takeaway is to explode things whenever you can, seems to work better!
    I found i had to have the hex pattern grouped to get the center line tool to do the whole thing at once, then i exploded it after and the paths came out simpler, took ~18min to cut.
    one pass, 0.2"DOC 1/8" two flute upcut carbide endmil, 45ipm, 3 speed on the Makita.

    Regards
    Gary
    IMG_3322.JPG
     
    David the swarfer likes this.
  13. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    No, do not always explode the holes!
    They are created as groups because of interference from lines that are underneath the holes (a special Sketchup 'helpful' feature). If you ungroup them with the wrong kind of line underneath them, you will get some 'interesting' results. (details in the manual!)

    However, for a big grid of holes, yes, explode them and make sure there are no underlying lines. This will give the shortest cut time.
    you can also just select all the lines by triple clicking one of them.
    that will select all connected lines. then apply the centerline cut.
     
  14. Gary Bonard

    Gary Bonard Well-Known
    Builder

    Joined:
    Feb 11, 2015
    Messages:
    8
    Likes Received:
    1
    Hi I'm new to the sketchucam , will cam sketchUp on Mac?
     
  15. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Yes
     
    navyto likes this.
  16. navyto

    navyto New
    Builder

    Joined:
    Apr 21, 2017
    Messages:
    2
    Likes Received:
    0
    Hello David,
    I started using sketchucam. I think I read and watched all the tutorials I found in google. I need to make inclined surface, sth like a ramp, but can't find a way to do it. Please help. Thank you!
     
  17. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    880
    Likes Received:
    172
    Making a ramp like surface is more 3d machining than 2d machining and SketchUcam doesn't handle 3d machining very well. BUT...it can be done if you go a little bit through hoops. There is an option for cutting 3d in SketchUcam but read the help file on how to do it. You may have to do the ramp separately from the rest of the part.
     
    David the swarfer likes this.
  18. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    The reality is that a ramp is 3D machining which is mathematically challenging (-:
    We have a 3D module but it fails to use the correct bit diameter offset and since it is uncommented code I have not yet been able to figure out what it does (and/or does wrong) in order to fix it.

    For a simple ramped face you can try doing it manually.
    If you pocket the face with the cuts running from top to bottom of the ramp you can then manually calculate the coordinates for the ends and then search and replace in the gcode file to implement those Z heights.

    So, for a simple face we get this Gcode, this is a zigzag only pocket 100% deep on 20mm material, I have added comments to explain what it is doing
    Code:
    %
    G90 G21 G49 G17 F1000
    M3 S30000
    G00 Z5.000
     X11.050 Y11.063     ; go to start position, bottom left corner of face
    G00 Z0.500                   ;descend just above surface
    G01 Z-20.000 F1000    ; plunge to depth
     X58.950 F2000              ; cut to the right
     Y13.679                        ; move Y up
     X11.050                       ; cut to the left
     Y16.295                      ; move Y up
     X58.950                 ; cut right
     Y18.911     ; and so on
     X11.050
    G00 Z5.000
    G00 X0 Y0 (home)
    M05
    M30
    %
    
    now, if we want a left to right slope, the left hand end of all those cuts must have a different Z height (0, top of material), and we must also then make we tell it what Z to use for the right side (-20 in this example).
    Code:
    %
    G90 G21 G49 G17 F1000
    M3 S30000
    G00 Z5.000
     X11.050 Y11.063   ; left side start point
    G00 Z0.500
    G01 Z0.0 F1000    ; left side height Z0
     X58.950 Z-20 F2000  ; to to right, Z down to -20
     Y13.679
     X11.050 Z0    ; cut to left, Z up to 0
     Y16.295
     X58.950 Z-20  ; cut to right, Z down to -20
     Y18.911
     X11.050 Z0   ; cut left to Z0
    G00 Z5.000
    G00 X0 Y0 (home)
    M05
    M30
    %
    
    so, not hard to identify the numbers and then search and replace.
     
  19. navyto

    navyto New
    Builder

    Joined:
    Apr 21, 2017
    Messages:
    2
    Likes Received:
    0
    Thank you very much for the quick response!
     
  20. davdue

    davdue New
    Builder

    Joined:
    May 5, 2017
    Messages:
    5
    Likes Received:
    0
    I have a part that I am trying to use SketchUcam on. It has a couple slots. When I use the outside cut tool it wants to make the part into 3 pieces (cut along the slot) rather than the outside line. Attached is a jpg of the part. I tried drawing a line from each corner and that didn't help. Any ideas? Z Axis Carriage Bottom Plate.jpg Z Axis Carriage Bottom Plate.jpg
     
  21. Giarc

    Giarc Master
    Builder

    Joined:
    Jan 24, 2015
    Messages:
    493
    Likes Received:
    234
    How wide is the slot? Is it the width of your end mill? If so, use the slot cutting tool in sketchucam. I made slots in a project that were wider than my end mills so I used the inside cut tool and drew a rectangle where I wanted the slot. Then I lied and told Sketchucam that the material thickness was the depth of the slot I wanted. I had to make more than one gcode file, one for the slot and one for the actual cuts using the correct material thickness. If I remember right, I may have made the slot gcode drawing file slightly longer than reality to make sure the slots were cut all the way to each end. It worked, but there is probably a better way.
     
  22. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Craig you did it correctly (-:







     
  23. davdue

    davdue New
    Builder

    Joined:
    May 5, 2017
    Messages:
    5
    Likes Received:
    0
    I don't think you are understanding my problem. I have no problem getting the slot or pocket to cut. It is the outside cut that has the problem. Here is another example I have shown it in isometric view. The top left part has been flattened and I have used the outside cut tool. The top right part has not been flattened so you can see what the pocket is supposed to look like. I have drawn lines across the top also drawn a rectangle where the outside cut sneaks into the part. Neither worked. If i draw a line across each opening at the top the pocket tool will work just fine. I am using SketchUcam 1.4d
     

    Attached Files:

  24. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    880
    Likes Received:
    172
    davdue, make the inner parts, the one that cause the outside tool to go inside, a group, including the pocket, and it will not happen anymore.
     
  25. davdue

    davdue New
    Builder

    Joined:
    May 5, 2017
    Messages:
    5
    Likes Received:
    0
    JustinTime,

    I tried several ways of making a group of the inside items and also making the outside line a group but they all do the same thing when I try the outside cut. Below are the items I selected for a group and then the group selected as well as the Sketchup file. Any more ideas?
     

    Attached Files:

  26. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Watched the videos?
    Understand the concept presented of creating copies of the part, each copy used for a different part of the Gcode generation?
    There is another video on my channel, the Seatknob Project, that goes into more detail and uses 5 separate copies of the drawing to get the article made, but the sound is bad so I don't normally recommend it.

    I would do this:
    1. copy the part.
    2. on copy one do the pocketing and anything else needed
    3. on copy two do the outline, removing any lines that cause problems with creating the outline cut.
    4. generate Gcode for each part making sure to register the safe area properly as detailed in the videos (esp the 2.5D for 3D parts one).
    5. join the Gcode files with the Gcode joiner.

    Why do we have to do this?
    Because Sketchup always splits lines that intersect, we cannot prevent it except by messing with grouping and that does not solve every problem. Intersecting lines are followed to create the outside cut, even when they go the wrong way to our eyes. Internally there is only math, no 'picture' of what we want.
     
  27. davdue

    davdue New
    Builder

    Joined:
    May 5, 2017
    Messages:
    5
    Likes Received:
    0
    Thanks David that makes sense. I watched the first one. I have a problem understanding the videos without sound. I guess they go to fast. I will try to watch them later when I have a little time to start/stop them and try to follow along. These parts are for a Joes2006 router. I am hoping to find a place to cut these parts (either our high school) or maybe I will have to join a local makerspace.
     
  28. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Just pause the video to give yourself time to read and follow the mouse cursor. If I leave the text on the screen for 'plenty of time to read' the video would be 3 times longer and no-one would watch it at all. I recommend watching it end to end, then watch it again, pausing as needed. The alternative it read the entire manual. Your choice (-:
    (why are some of my videos silent? because I don't have a microphone on all my computers so it just depends which one I am using, and adding sound afterward in Windows Movie Maker just plain sucks)

    Attached find your updated file. I have added the copy for the outline cut. Added hole drilling, and added the pocket cut at 100% deep. I also changed the tab size, they were too small.

    This means you need to generate 3 gcode files.
    1. put the safe area around the left hand stuff
    2. set the material thickness to the depth you want for the pocket, select the pocket and generate file1
    3. set material thickness to 0.5", select all the stuff in the safe area, then DESELECT the pocket, generate file2
    4. move the safe area to the right hand marker, generate file 3
    5. use the joiner to join the files in order
    I recommend adding a 4th file of just the holes and use an actual drill bit to drill them before doing the rest of the cut. Do not join the hole drill file with the rest of the files. The reason is that router bits do not drill well and tend to get clogged up when plunging straight down.

    Also, please turn off fractional inches and use decimal inches instead (and use 4 digits of precision). You can still enter fractional numbers in any Sketchup edit box, Sketchup will translate it correctly to decimal inches. Sketchup has bugs in the fractional processing (of things smaller than 1/16") that will bite you at some point so better to get used to not using it now.
    (in fact you can enter millimeters when in inch mode, just enter '10mm' and Sketchup will translate it)

    If you are making these parts out of aluminum then:
    • definitely drill the holes before milling the rest
    • turn on ramping
    This is what my file will cut, the pocket is 0.15" deep
    Z-Axis Layout 36X34 1.png
     

    Attached Files:

  29. davdue

    davdue New
    Builder

    Joined:
    May 5, 2017
    Messages:
    5
    Likes Received:
    0
    David,

    I watched your "Cutting Text with SketchuCam" video. How do you control the depth of the outside and inside cuts? By changing the material thickness and inside/outside overcut percentage?
     
  30. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    644
    Likes Received:
    306
    Inside and outside cuts are normally 'through' cuts with overcut% greater than 100.

    However if you want to just outline the text, then set overcut to 100% and set material thickness to the depth of cut that you want.
     

Share This Page

  • About Us

    The OpenBuilds Team is dedicated helping you to Dream it - Build it - Share it! Collaborate on our forums and be sure to visit the Part Store for all your Building needs!
  • Like us on Facebook

  • Support Open Source FairShare Program!

    OpenBuilds FairShare Give Back Program provide resources to Open Source projects, developers and schools around the world. Invest in your future by helping others develop theirs!

    Donate to FairShare!