Welcome to Our Community

Unlock hidden features. Sign Up for Free Today!

Sketch U Cam Not Creating All of the G-Code

Discussion in 'CAM' started by n0kjf, Sep 22, 2015.

  1. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Help please,

    I am trying to cut some table center pieces for a club meeting this weekend and Sketch U Cam is not creating the G-Code for the out side of the dog. All other G-Code seems to be in place.

    What am I doing wrong?

    Thanks, Lew
     

    Attached Files:

  2. Flash22

    Flash22 Veteran
    Builder

    Joined:
    Sep 1, 2015
    Messages:
    109
    Likes Received:
    28
    I selected all and then did a blrepair and phlatten (24 lines repaired)- reselected the cuts and it seems to have done it
     
    n0kjf and David the swarfer like this.
  3. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    apart from non-flat drawings causing issues....

    there is a problem with complicated outlines, the offset routine that creates the cutline can get confused by short segments and sharp internal angles in such a way that it creates little 'spikes' on the cutlines, at corners. this in turn prevents it creating the face between the object and the cutline, which prevents the Gcode being generated from that line.

    so, if some cuts get left out, look for tiny spikes on the cut line, remove them, and create the face.

    There is a nice plugin called 'EdgeTools2' that will simplify a complicated outline, such as one might get from converting a scanned image to vectors, that helps greatly in solving this sort of issue.

    There is also a small plugin that can highlight such spikes, stray_lines.rb is what it is called. Google for the download.
     
    n0kjf likes this.
  4. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Thanks Flash, I do not seem to be able to make it work for the dog's exterior, or the larger interior cut. I get the 6 lines repaired, but I cannot get the correct g-code for the entire drawing. The line cuts have the z retracting between line segments instead of making a continuous cut. I've tried the fold and the center line, both do the same. :(

    Thanks,
    Lew
     
  5. Joe Santarsiero

    Joe Santarsiero OB addict
    Staff Member Moderator Builder

    Joined:
    Oct 30, 2014
    Messages:
    648
    Likes Received:
    135
    Are there any features where the cutter diameter will not fit?
     
    n0kjf likes this.
  6. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    No, at least I don't think so, I went around all of the ins with a circle larger that the 1/8" bit to make sure it would fit.
     
    Joe Santarsiero likes this.
  7. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Mark sent a file to me that will work, I'd still love to know where I'm messing up for future reference.
     
  8. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    772
    Likes Received:
    152
    Lew, the reason you don't have the outside line cut is that when you generated the outside cut line no 'face' was created. If Mark sent you a fixed file, click on the space between the outside cut line and the part. You'll see that it is a 'face'. That's the first thing I check when I don't get an outside line to show in a plotter.

    When I have that problem I start drawing lines like in the attached picture and I create a face. I continue drawing lines until I get to a place where I can't make a face. I didn't do your whole dog, just the portion that you see in the pic, and I already run into a problem. If you zoom into the red outline you'll see that the outside cutlines in this place are not touching. I don't bother to find out why they don't, I just take the move tool and connect them. Faster then trouble shooting it. Once I fixed it I make a face in this section. I go over the whole thing until I have it all in a face. I then erase all the little lines I made and generate the g-code.


    Untitled.png
     
    n0kjf likes this.
  9. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Ok, Thanks, the bone tool messed me up. It was my first time using it.
     
  10. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    That works well, the only issue I have left is cutting the interior lines full depth. The g-code cuts them as small segments and z's up to safe travel and plunges back down..wasting a lot of time.
     
  11. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    For the interior line, it is almost as if it is perforating instead of cutting a continuous line. I'm so close...
     

    Attached Files:

  12. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    If I offset the line and make it a "box", I can do a out side cut. The issue is the the line becomes 1/4" wide instead of 1/8".
     
  13. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    I have just looked at your file and found the following:
    your radbones are too small. you have the bit set to 0.125" and when I click the 'phlatbone tool diam' button I get prompted with 0.135".
    I accepted that and redrew the radbones and then the outside cut tool applied perfectly, first time.

    The help for the phlatbone tool diameter button says:
    Tool Diameter -
    ALWAYS CLICK THIS BEFORE USING THE PHLATBONES TOOLS!
    This allows you to set the tool diameter that the Bones tool will use.
    This version of PhlatBone tools is integrated with SketchUcam.
    This allows it to fetch the current SketchUcam tool diameter and present it as the default in this dialog.
    0.01" will be added to the bitdiameter to allow space for the inside or outside cut.
    In some cases this allowance will be too small and you will need to redraw the bones with a larger diameter. In many cases the generated inside/outside cut lines will contain very small arc segments which can confuse some controllers. If this happens remove the cutlines, select all the bone arcs, right click and select 'Explode Curve' . Now when you add cut lines they will be much simpler, containing only straight line segments.
    Alternately you can use a larger diameter for the bones.


    (a note: that needs editing since all phlatbones curves are now created 'exploded' and with just a few segments which largely solves these issues, except when the offset is too small!)

    The centerline cuts that are cutting in 'reversed segments'.... this is caused by the order in which the lines were drawn, and then side effected by the order in which Sketchup gives them to SketchUcam for processing. What you need to do is create a break in the line where the reversal occurs, so that you effectively have 2 separate lines, each with the segments all drawn in the same direction. I created a 0.01" split at the reversal points and now the Gcode generates perfectly.

    You can also try the Bezier Curves plugin and select 'convert to polyline' before setting them as centerline cuts. This resets the line directions most of the time. Sometimes it does not work and you have to just split the line and move on.

    I could not find mention of this in the help so will add it! That is a very old section that has not changed since version 0.8 or so (-:

    I have attached your corrected file.

    BTW there are a lot of tiny line segments in the drawing, many around 0.001" long. Using the EdgeTools2 plugin to remove those short segments would be of great benefit. Loading and saving the drawing would be quicker, adding cutlines would be much quicker, and cutting the Gcode could be 5 to 10 times times quicker. You don't need line segments that are shorter than about 1/5th of the bit diameter.
     

    Attached Files:

    n0kjf likes this.
  14. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    772
    Likes Received:
    152
    The reason it does it is that the drawing calls for, I think, CW direction but the SketchUcam script wants to make it CCW (for the outside cut)! That happens if you flipped the part AFTER you made the cut lines or if the 'face' is reversed.
     
    n0kjf likes this.
  15. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    it has nothing to do with the face and everything to do with the way the lines were drawn or edited, how Sketchup stores them, and how it gives them to SketchUcam for processing. splitting the line where it first reverses is a total fix.
     
    n0kjf likes this.
  16. JustinTime

    JustinTime Master
    Builder

    Joined:
    Dec 18, 2013
    Messages:
    772
    Likes Received:
    152
    I made a circle. I copied it and reversed the face of the copy. I generated the outside cut lines. I had to use the shift key on the reversed face copy since it wanted to generate the lines inside. I generated the g-code it the copy comes out stitching the original, without the reversed face is OK. Is this because I used the shift key?

    Untitled.png
     

    Attached Files:

    n0kjf likes this.
  17. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    I wonder if part of the issue is the original drawing was in AutoCAD and imported into SketchUp. I know that arcs don't import correctly at all. I tried the Weld plugin to make the line contiguous, the center line and the fold tool breaks it back into tiny segments.
    Dave, when I get back home, I'm going to try to reproduce your results, I'm sure I'll need to use it in the future projects. I have a hard time drawing in SketchUp, I miss having the offset tool for instance. I can use the offset tool in AutoCAD on complex curves, I have never caught on how to do that in SketchUp.
    I did add the EdgeLines2 Plug in, and I was playing around with it.

    I'm going to show up at someone's doorstep and camp out until I learn all the tricks. Ultimately I cut the dogs out without the inside lines and everyone loves them, we gave them out at a Eurasier dog get together this afternoon. We had 14 dogs. and 8 families show up, it was fun.

    Thanks for all the help, I'll be back with more questions I'm sure. I really appreciate all the help.
    Lew
     
  18. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    that is quite clearly broken! outside tool must apply to the outside of a face otherwise the arc processing gets broken. you could work around it by exploding the arcs before applying cut lines.

    in fact this is so broken I have jut removed it from the code for the next release.
     
    n0kjf and Joe Santarsiero like this.
  19. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Hi Dave, I'm back home and looking at trying to learn this stuff for future reference. For this project, I gave up on the interior cuts, I was out of time. I attached a picture of what I ended up with. Everyone loved them, we gave out 11 to our fellow Eurasier owners.

    Anyway, where can I find the Bezier Curves plugin? There are several options in the warehouse, I want to look at the correct one.

    What is the best way to find the tiny line segments? I drew the original in AutoCAD and the lines do not seem to import well, a lot of the curves end up as truncated line segments.

    I drew the bones in the AutoCAd drawing, I had a hard time understanding what the size of the tool was doing for me. I assume it is the diameter of the tool and I thought I'd hedge a little and set the size to .135", hoping the bone would be large enough to work. I'm cutting with a .125" tool.

    When I cut foam, I typically use a lot of tabs, knowing I can buzz through them with an Exacto #11. When I'm cutting wood, I use a lot less tabs. I have been playing around with getting g-code to cut just the tabs. That would be a nice feature to add. I got the idea after playing with Justin's pointer about drawing the line to track down the breaks. When I was doing some erasing, I left a section of outside cut, being curious, I converted to g-code and it did show a short cut where the cut line is. Hmmm, I can cut just the tabs using this trick. This would be a nice future feature.

    Thanks a lot for the help.
     

    Attached Files:

  20. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    looks good!
    This is the one
    http://sketchucation.com/forums/viewtopic.php?t=13563
    use the 'convert to polyline' option after selecting all the line segments you want contiguous. do note that sometimes it just doesn't make a difference to the cut order, and then you can just do the split technique I showed you earlier. a 0.25mm split is not visible with a 1/8" bit (-:

    Edgetools is this one
    http://sketchucation.com/forums/viewtopic.php?f=323&t=24593
    the tool to use is the 'curve simplification'
    I used to do it visually, just zoom in and scroll through the whole length of the line to see them, but recently I foudn this plugin
    http://www.smustard.com/script/StrayLines
    that can quickly highlight them for you.
    NOTE that it will highlight the ends of any line that is not a loop, that you still want, so do not use the 'delete all', rather use 'select all' and then zoom in to each one to decide what to do with it.
    ah, the joys of DXF >-: exporting your DXF without arcs works better.
    Rather do the bones in Sketchup using the phlatbones tools. first click the 'tool diameter' icon which will automatically add an offset to your current tool. I measured your bones to be less than 0.135, but they also had more segments than the phlatbones tool inserts, and that is part of the problem. a few versions ago I spent a lot of time on the phlatbones tools to make them more reliable, reducing the number of line segments, exploding the arc, and figuring out an all round 'works mostly' offset.

    The issue is that offsetting the cut lines inside a small area such as created by bones is geometrically 'hard'. give it a try with the built in sketchup offset tool and you will see that it does the nuttiest things in sharp corners.

    the SketchUcam offset routine does much better, but can still go crazy on small internal arcs, which is why the phlatbones tools do not create arcs any more, use just a few segments, and have to have a proper increase in bit size to allow some space for the offsetter to do its work.
    No feature needed (-:
    Simply because you can very quickly create a copy of your drawing and apply an outside or inside cut to it with no tabs, set multipass off and do a single fulldepth cut through all your tabs. you can even up the feedrate since your tabs can be pretty thin so the cutting forces are low.

    Sure, if you are cutting hundreds of parts you may want to optimize this to only cut the tabs off. I would do this by (on a copy of the drawing) adding an offset line, trim that to only the bits that would cut through the tabs, then 'centerline cut' them at 100% depth.

    So, having read the help, at least the 'toolbar help' which explains each of the tools and the 'options' help, you will learn a lot by watching my videos:
    the basics

    the multiple drawing technique

    using ramping, this was added for aluminum cutting but has proved to be really nice for just about any material.
    adds time so don't bother on foam though, unless you have a 3 tooth downspiral bit like mine, that will melt the foam when plunged too fast.

    and then, the multidrawing technique in action, with ramping too.


    have fun
     
    Firetruckguy and n0kjf like this.
  21. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    Wow, I've been studying this wealth of information, Thanks.

    I was able to get most everything done much easier now. More tool and know how. I'm still playing around with the drawings just to learn.
     
  22. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    I finally got it! :thumbsup:

    The bad news is that I needed to be here with the g-code last week. The good news is that the club is going to put the Eurasier dog on their website and sell it as a fundraiser. So anyting I cut in the future will have the interior lines cut in as well.
    David, your information is awesome thanks for your patience and guidance.

    I've always had a little trouble holding the part in place while the tabs are cut. So I followed your suggestion of offsetting the line and doing a center line 100% depth cut. That worked very well for me. I don't plan on cutting 100's of these like I cut of the foamies, these will probably be in ones and twos. Still, it was good practice for me and I did learn a lot.

    I used the PhlatBone tools, Edge Tools², Bezier curves tools. I might start drawing everything in SketchUp now that I have some tools and knowledge to work with.

    So here is what I did to fix the interior curved center line cuts.

    1. Draw the curve.
    2. Select the entire curve and Weld.
    3. Select the entire curve and RepairBL + Phlatten
    4. Select the entire curve and Stray lines; delete Using the plugin from David's post.
    5. Add a short straight line at each end of the curve.
    6. Select the entire curve, apply the center line tool.
    7. Select the entire curve and create g-code, and view to verify it has worked.

    Anyway, this is what worked for me.

    2015-10-01 18.12.03.jpg
     
  23. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    Very nice!
    Boils down to knowing your tools (-:
    Know your hammer, you can hit anything with it, successfully.
    Don't know it, all you can do it tentatively tap on a nail.
     
    n0kjf likes this.
  24. n0kjf

    n0kjf Well-Known
    Builder

    Joined:
    Feb 10, 2014
    Messages:
    18
    Likes Received:
    3
    SketchUCam hates me. Really hates me.
    Sketchup 2016.

    So, load the Sketchup file, there are 3 pairs of curved lines. Use the center line cut tool on the right line of each pair. Create g-code... test 01.cnc. Then again use the center line cut tool on the other 3 lines and create g-code. text 02.cnc.

    Why is that happening??? Specifically, by selecting the center line on the left curved line of each pair, the right cut line segments....
     

    Attached Files:

  25. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    524
    Likes Received:
    251
    ah yes, the old line presentation order thing.....
    you drew the left hand line 'going up' and the right hand line 'going down' (or down/up), and sketchup remembers that line order, but does not convey that information to SketchUcam.

    to fix...
    apply cuts to all 6 lines.
    select the 3 right hand lines and 'create group'
    optionally select the 3 left hand lines and create group
    generate gcode.
     
    n0kjf likes this.

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!