I thought 'oh, cutter compensation is on' but then realized that would affect the size rather than just an X offset. I read you gcode into g-code-ripper and converted it to dxf, and the dxf comes out correct. I red your original dxf into Sketchup and it is correct. So now I want your Sketchup file so I can generate and run gcode directly from it on my machine.
I just ran both files of code through my machine and it cuts perfectly with everything centered as expected. I cut both files with the same 0 settings and they cut exactly on top of one another. (I did change the feed rates though, from F200 to F1900 so it would finish today I highlighted the edges of the foam with Sharpy so they can easily be seen... displayed in bCNC so now I think you have a Mach3 problem (assuming it is not hardware).
Hi Firstly, thank you for all the effort you have gone to, I have attached the SketchUp file. I will take a look at Mach3, you may be correct in saying that it is causing the issues, I have been getting some issues whilst running the machine, but thought it might be the pc, not coping.
if you have not tuned Windows for Mach3 according to the instructions on the Mach website then you WILL have problems. maybe not THIS problem, but problems nevertheless. Windows is not built for running realtime tasks and so Mach has a hard time doing it, so we have to make it as easy as possible. Kill every possible background task, remove unneeded software, and so on, the machine has to be dedicated to Mach3, no compromizes.
Hi, I need your help on the problem i'm having in SketchUcam v1.4d, and it's a really simple drawing. I am drawing in sketshup the two semi circles only, i use cut outside tool, and when i see the g-code always makes a complete circle out.
Hi The way Sketchup cuts off the ends of arcs can be a problem for Gcode generation because the centers get lost. The way to fix it: remove the cut lines right click each arc and select 'Entity info' in the Entity Info change the 'segments' to 48 or 96 (or any multiple of 12). (increase it until the arc segments are about 2mm long.) press enter right click the arc and select 'Explode Curve'. Now the arc is not arc segments but small lines, thus voiding the truncated arc segments that Sketchup generates.
Thank you for the great help and quick response, already tested and worked well. We are always learning and who knows know Thanks again
Hi, I am having a few issues using duet3D wifi and the attached gcode exported from SketchUcam. When using the plotter or ncviewer everything looks good Some of the errors I get are shown below, any ideas? This is my first CNC project by the way so complete newbie! Error: Bad command: % Warning: G49 command is not supported Warning: G17 command is not supported Warning: M3 command is not supported in machine mode FFF Error: Bad command: X58.900 Y55.820 Error: Bad command: X57.537 Y57.439 F2000 Error: Bad command: X56.479 Y59.341 Error: Bad command: X55.729 Y61.528 Error: Bad command: X55.310 Y63.864 Error: Bad command: X56.618
% is the standard 'start of tape' symbol, if duet does not like it, just delete it G49 is turning off tool offsets G17 is setting the work plane to XY M3 is trying to turn the spindle on (go to the duet website and find out what mode FFF is and how to change to a mode where you can turn the spindle on) the rest is because the Duet is expecting a modal command (G0 G1 G2 G3) on every line, which is not how Gcode normally works (the definition of 'modal' is that it gets remembered so you dont have to repeat it on every line!). You can get those commands on every line by turning on 'all codes for Marlin' Described in the user manual for SketchUcam which is already installed on your computer and is also at SketchUcam: HOWTO set default options\ Also, if you are cutting anything harder than foam you should turn on ramping. Just default it on, I use it for everything. And you want to set Sketchup to millimeter mode, meter mode is not tested so I cannot guarantee that the options dialog will work properly)
oh I see thanks very much! I use a dewalt d26200 which is not controlled by the Duet (I manually set it on/off and speed by hand), is there a way to set this to manual so the gcode doesn't export any spindle on/off commands? I would like to cut various materials once I figure out how to use it properly but mainly MDF/Acrylic I set it to mm mode now and I reattached the test file. Any further help would be much appreciated.
Although the Duet is not actually controlling the spindle it should still be able to accept and process spindle on/off commands, just like every other controller does. Some controllers will not even move unless they get a spindle on command. Thus, there is no way to not emit spindle control codes, it is just never needed. You do need to visit the Duet web site FAQ or forums and also read the user manual. Knowledge is power (-: I do not have a Duet so I simply cannot help any more with its specific settings. There is nothing wrong with the gcode at all, I could run it through my machine right now without any issues. However, when you come to do an inside or outside cut you will want to set the bit diameter correctly, 6350mm is a tad on the large size (-: And you will want to learn more about SketchUcam too, you have the manual but maybe the videos can help a little SketchUcam Howto - YouTube
So... anyone keen on this.....(watch the attached video) Working in Sketchup Make 2016, should work from Make 2014 onwards, sadly not in Sketchup 8
I've been using SketchUCam for a few weeks now and getting a handle on it. I've been a sketchup user for at least 10 years so a lot of it is pretty obvious to me and I can see how the SU environment makes it tricky for SUCam. I have to say that SUCam works pretty nicely over all. Probably my biggest complaint is how SU "demotes" circles and arcs to segments if you look at them wrong (though it's mostly predictable). Not sure if the SUCam code can do anything about that. It does mean you need to look at how you convert your sketchup design so SUCam can do a decent job on it. I have a design that had 2 parts with identical 70mm holes with a cut in the side (so, they were about 330 degree arcs). One remained an arc and the other was converted to segments (I used 96 segment circles to start). I have no idea what I did differently between the two. Made the mistake of not checking both - looked at the first and it was an arc so assumed the other was too. The first part took about 8 minutes to cut on my CBeam and the other took 40 minutes. Because of the 96 segment circle the part was usable. If I do it again, I'll probably generate GCode for the circles separately and combine with the rest of the design. On a different issue. I can't seem to get save/load parameters to work. Well, it does appear to save them but when I load it doesn't appear to load all of what I saved. Safe area never changes, for example.This is with SketchUcam V1.4d-80c0152 on Win 10.
Using layers with SketchUCam. This works but it would be really cool with one change. Currently it appears that all layers are used to generate GCode, even ones with "Visible" unchecked. If only visible layers were used to generate GCode, then we could use this to separate out pieces of a design for different treatment. I'm probably naive to think that it's as simple as a check to see if visible when generating code for a given object. This could make for some interesting enhancements: - attach different parameters to a give layer - tool change. put all the cuts with given tool on a different layer.
an interesting proposition, BUT..... from the Sketchup reference We already have problems with generating lines that get interfered with by existing lines, how much worse if that interference is from things that are invisible! While I will look into the use of layer visibility I will say that for now the existing system of using groups and multiple drawings does work very well. While gcode is generated for everything inside the safe area by default, if anything is selected (lines/areas and/or groups) then Gcode is only generated for the selected items. If you don't yet know how to use the multiple drawing technique then here is a video:
This help page tells you what the tool profiles save (also installed on your computer, hit the big blue question mark in the toolbar). SketchUcam Toolbar
Yes, I watched that. The problem I have is keeping track of multiple of the separate items that need to be aligned properly and what specific parameter apply to each one. Thanks for your help. Would you prefer SUCAM posts here or on github?
I use the label tool pointing at the origin for this drawing and put the reminder I need in the text portion. In this drawing I just labelled the top corners but you get the idea. I am using a new method for multipart drawings so the labelling of the origin point is not needed in this drawing. Would you prefer SUCAM posts here or on github?[/QUOTE]
Yeah, started using labels like that last week when it became apparent that the complexity was getting hard to manage. I also added the the name of the individual file to keep that part straight for later combining. pocket1 gets saved in 6mm-pocket1.cnc for example. Your technique looks like you copy the entire object, reset the 0,0 origin and/or safe area point, make the changes needed and then add the cut. Might be a bit easier to keep straight. Though, I wish each cut "object" could be given attributes like depth and tool diam. That could reduce the number of files needed.
labelled tags like that are exactly what I am talking about. my old method involved making multiple copies of the drawing at regular offsets and using a construction line to define the 0,0 point, then moving a suitably sized 'safe area' box from point to point to select what gets generated. recently I have been doing it differently. I still make copies of the master drawing but they can be at any spacing and do not need a constant offset. The safe area is left as the same size as my machine and encompasses all the drawings. I then pick a constant feature within the drawing as the 0,0 point and use the zero point tool to set that as the origin for each drawing in turn. I then select the stuff to be cut with the selected origin and generate Gcode. In this way one origin can be used for more than one set of cuts, for example one of the drawing copies may have holes AND pockets on it but by selecting just the holes and a generating and then just the pockets and generating that one drawing can serve 2 purposes. This is handy for very precise depth pockets. Set the pocket to 100% deep and then set the material thickness to the exact depth you need. Yeah, I need notes to keep track of what goes with what but that is normal. I also sometimes generate a hole drilling file with just 0.5mm material depth which really just marks the surface. I run this (with a real drill bit) and then use my electric screwdriver to drill the holes through before running other code. I do this mostly on polycarbonate plastic which gets hot and melts very easily when drilling so a pilot hole is very helpful.
I'm trying to "engrave" a pattern with straight lines and arcs. See the attached image. My first thought was to use the centerline tool. It works but doesn't use arcs, instead converting the arcs to a sequence of segments. What I want is essentially an inside (or outside cut which uses arcs) with a zero offset. I tried defining my tool as having zero width but that gets "smacked down" (half inch bit gets used, lol). I want my toolpaths to use arcs, is there anyway to do this?
the centerline tool cannot output arcs. (nor can the pocket tool) what you can do is select each arc and set the number of segments 'high enough' before exploding the curve into segments. 'high enough' depends on the scale of the drawing. you want the resulting segments to be shorter than the actual bit diameter. you can just do some trials by setting the segment count and then measuring a segment, repeat until happy with the length. but beware, if you scale the drawing up the segments may become noticeable in the cut, so only do this to the final size drawing.
Yeah, I knew that was the most likely workaround but there are cases where SU won't allow me very many sides in shorter arcs. There are several like that in the drawing I posted. There's one that is 16mm long - SU refuses to allow more than 3 segments and it is fairly obvious when I cut it. Is there a reason you don't allow a zero offset for inside or outside cuts?
Yes, there has to be at least 0.001" between all points on the object and all points on the cut line. so the minimum tool diameter is 0.002" and there is no guarantee that it will work at that size, will probably have to be bigger to cater for diagonal differences that are less than 0.001414" (square root of 2, because 'math').
Hi Was wondering if there is a way to set a drill gcode in sketchucam rather than cut the holes with a router bit. I have about 25 holes is two different aluminum plates I need to drill any help would be appreciated. Thanks Brian
David can give the definitive answer but if you select a bit the same size as your hole it just plunges. You can also select peck mode if your hole is deep.
By the way, I have been using a v-bit to just mark the holes (.2mm deep) and then drill them on a drill press. Allows me to use arbitrary size drills as well as drills that are smaller than my smallest bit.
