I have just stumbled on phlatscript today (yay wow awesome etc - now I must build the machine).
and today I have solved the metric gcode problem (though I haven't bothered with the constant changes you made, yet - seems to me to be code needed in the setup dialog to allow a choice of output mode).

Anyhow, compare your phlatmill.rb with the one at
http://iwr.ru.ac.za/~david/phlat/
and insert the 'tometric' bits. You can ignore the changes I made to make TurboCNC happy with the code (yet to be tested)

Thing is, Sketchups native internal units are imperial, no matter what is displayed on the screen.
I have modded it so it converts anything being 'output' to millimeters,leaving all internal math alone.

If the writers of phlatscript want to make use of my code they certainly may. I'll probably do more mods when my machinery come online...

 

What I did was leave all the internals in the native inches, and only convert for output.
If there were a 'metric' checkbox in the setup, my 'tometric()' method could query that to determine what to output. Leaving the internals alone removes one level of floating point fuzziness which is 'a good thing'

I had a quick look yesterday at the code, thinking to add a checkbox to the settings dialog, but I ran out of time. Maybe I'll drag the laptop home and see what I can come up with.
Ultimately one would need to ask Sketchup what the display units are and act appropriatlely, but also allow the user to work in inches on the screen, but output metric gcode. This will give greater accuracy on a metric leadscrew machine. Here in South Africa, it is impossible to buy anything but metric (my Myford lathe is imperial and I am comfortable with that) so any machine build will be metric.

 

Hopefully you havn't gone too far with that. On Saturday I sat with the laptop and made extensive changes to 4 files, which replace what I did on Friday.
The dialog has 2 checkboxes added as you can see here


Also, the code will detect metric mode and output metric gcode if the drawign is metric.
The 'Force Metric' checkbox will enable metric gcode no matter what units the drawing uses.
This should actually be a radio button collection to allow 'Force Imperial OR Force Metric' to be selected, or none (but I coudln't figure out how to do that without manuals).

The 'TurboCNC' check box enables gcode that is friendly to TurboCNC, which doesn't understand G49 and maybe other stuff, though a test file I ran through it was ok, I may find other stuff when I start cutting complicated shapes etc.

The dialog still has an issue in setting the default values. Though I put in code to selected the metric default values for bit diameter etc when the drawing is metric, they still come up as 1/4". Strangely, the same sort of selection code works for the safe width/height settings. Pressing the 'restore defaults' button will set the bit diameter etc correctly.

So, if you want metric gcode RIGHT NOW, install phlatscript 0.918 as per the instructions.
Once that is working, replace the existing files with my files on the web page listed above (not the .png).
Restart Sketchup, of course.

 

Can be done, but 920 has a lot of changes and at least for me has bugs (would not do an outside cut after some edits), so I decided to wait and see if there is an update in the next few days before merging the code. If you really want metric in the short term, for now you need to install v918.

I'll see what can be done....

 

Ok, I did a simple no choices conversion, it will output according to the drawing units.
Nothing fancy, if your drawing is metric, it will output metric, otherwise imperial.

Get it down the bottom of (do not get any other files from that page)
http://iwr.ru.ac.za/~david/phlat/

 

I thought I posted about it but it seems to have got lost. Sadly I don't have the sketchup file anymore as I didn't save it (yup, thought DAMN just after closing SU). What I did was draw several random shapes, in particular polygons with narrow internal angles to see if that corner problem has been solved. One was shaped like 2 fingers raised '/' 4 edges , and I did a cut inside AND outside on that one. When I did a gcode check in NCPlot the central point of the V crossed over, ie the outside cut went to the same point as the inside cut, crossing the actual drawn outline.
I went back to SKetchup and deleted both inside and outside cuts, drew an extra line from the point of the V and deleted it, and replaced the inside cut without problem. But then when I clicked the outside cut tool any shape I selected showed the cut line on the inside. I tried ordering edges etc, but it just stayed that way, even though I deleted edges and replaced them and a few other edits.

By the way during my quick metrification yesterday (always more fun than work!) I ran the resulting code through EMC2 in sim mode and I'm impressed with the smooth curves, now if only I can build a machine that cuts nearly as well I'll be happy. Note that I changed the resolution (and justification) of the output numbers, imperial gets 3 decimals and metric gets 2. You had %10.6f and I thought that may be needed for the arc interpolations but EMC was happy with those settings (it will often bitch about start and end points being at different radii if there is not enough resolution). 0.01mm is less than .5 thou, I don't think any of our machines cut to more accuracy than that (and certainly less repeatability?). 0.001 resolution in imperial mode is probably enough for most machines IMHO, but any user who needs an extra digit can easily mod the code where @resolution is set.

I changed the justification to make the gcode more readable 'to me'. It's just the way I like it
I need to be able to read it because I plan to add a DVD laser to the cutting head for writing part numbers, and I'll probably need to hand code some of that and will need to figure out where to do stuff in the code. The laser will probably be on the W axis parallel to the Z. Driving it down to get in range will hit a switch to turn it on, restract for off.
Maybe phlatscript can detect something like a 0% centerline cut and output the correct codes? I'll have to see when I get there, I have built the stepper interfaces and am busy testing motors (I have a collection of steppers from printers, up to Nema34 size), next I'll build a small 3 axis gantry router which will cut about 150x150x50mm, just to learn what not to do, then comes the 1200x700x150 cnc router.

 

hey, I discovered how to reproduce some of what I saw.

What I did
Draw the V shape starting top left, bottom middle, top right, top middle, top left.
do inside cut
do outside cut
the result is that the top portion of the outside cut shares an inside point with the inside cut.
Sure, you are unlikely to actually cut something like this, but this is a possible intermedaite step, having mistakenly selected inside, then select outside before deleting the inside cut.

Sketchup file http://iwr.ru.ac.za/~david/phlat/bug1.skp
screen dump http://iwr.ru.ac.za/~david/phlat/bug1.png

 

Hiya

Thanks for the info on the shift key, I may well have pressed it at some point who knows.

On laser marking. I looked at gcodeutil.rb and while I wasn't thinking of adding a new line marking style, I agree that that is the way to go. Detecting 0 cut depth could also work but would require some extra housekeeping to get the W axis to retract in the right places.
It could also be done in phlatmill.rb but a new line style is a much better solution.

DVD laser modules can do about 200mw which is enough to mark medium to dark surfaces if you move slowly. That is what CNC does best (-:
http://www.flickr.com/photos/audin/1244728357/

That shows the basics, but from what I've read so far a good constant current power supply is the way to go, else the laser diode will die. And don't forget a heat sink on the laser.

This will also require that a tool offset is set up in the CNC software, because the laser will be offset from the router, and the gcode must select that tool for each 'writing' move, and reselect the normal tool afterward.

BTW I notice that some of the menu items have disappeared, like 'set as centreline' and so on. Are those coming back? I found them very useful. Is 'phlatten edges' equivalent to 'order selected edges'? Going off to seak and read a readme file...