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
I selected all and then did a blrepair and phlatten (24 lines repaired)- reselected the cuts and it seems to have done it
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.
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
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.
Mark sent a file to me that will work, I'd still love to know where I'm messing up for future reference.
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.
For the interior line, it is almost as if it is perforating instead of cutting a continuous line. I'm so close...
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".
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.
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.
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
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.
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.
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
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.
I finally got it! 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.
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.
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....
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.
