SketchUcam

Well, I don't know how you are not seeing them, if you read the cnc file you will see 5 sets of code like

Code:

(plungeboredepth  DEPTH=0.15  DIAM=0.125)
G00 Z0.0197
G01 Z-0.15 F100
G00 Z0.0197
G00 Z0.125
(plungebore end)

and those are the plunge holes, no problem.
Which then looks like this in GPlot

the row of 5 little downward blue lines are the plunge holes.

 

Sorry, no light background setup, but you can adjust the line colors from the 'Plotter|Colors' menu to get the contrast you need:

I use CAMotics CAMotics when I want a real visualization but for most checks I use bCNC to step through the code, this shows the tool path but not the result of the path like CAMotics does. I also often make the actual cuts in insulation foam, just to see what it will really do before cutting the expensive plastic sheet or whatever the project involves.

 

I sleep during the African night, about 8 hours ahead of CST (-:

 

set your sketchup profile to 'achitectural' which i think will give you the same colors i have. in this scheme any flat sheet shape will have a blue side and a white side.
all SketchUcam drawing must have the blue side facing up in order for the cut directions to be correct.



so the shape i drew is pale blue
the outside cuts are orange with a white area between the final object and the cut line
the inside cuts are cyan with a white surface between the object and the cut.

if you have to have another color scheme selected then what I am seeing as pale blue is in fact the 'inside' surface.
so if you create a 3D cube the outside is a different color to the inside, in my case inside is blue and outside is white.
SketchUcam requires that 'inside' surface to be 'up'

 

That looks good!
I used a KF foil on a slope glider, flying wing type. Did not work well at all. It is now on the 'modify' pile to get a tail fitted. Some parts have been cut, now if I could just find them...

 

do not cut that file. (-:

Some parts are too close together and your tabs are not lined up, and too many in some places, too few in others.
The 1/8" slots in the 2 long pieces need to be expanded by 0.002" so that the outside cut tool can get in there. Just because it draws a line does not guarantee a good cut.
Sketchup rounds to 0.001" so the gap has to be at least 0.002"

The tabs:
On circles, use V tabs (press END to swap types) and bridge 3 adjacent arc segments, in 2 or 3 places around the circle, depending on size.This is the only time we place tabs next to each other.
On straight edges (which must be more than 1.4" apart for a 1/8" tool) place the tabs opposite each other so that they support each other.
On straight lines place only one tab, a single click. This tab will be 3/8" long (in your settings). The tool will remove a tool radius from each end so the resulting leftover material will be 1/4" long.
For V tabs (they cut faster) you need to make them longer.

Units. you have Architectural fractional inches selected, decimal inches to 0.000" precision works better. You can still enter measurements as fractions by putting an " after the fraction to tell Sketchup to interpret it as a fractional inch.

Attached is what I would do..... well, I would use V tabs everywhere but I put some in so you can see what they do.

As for saving, click the green arrow, confirm the filename and folder and it saves, then gives you a dialog saying 'output saved to blah/blah/path/filename.nc'. After that you may need to click on any face in the drawing to let the Gplot previewer popup, some versions of Sketchup need this. I had no problem saving the gcode.

 

The tabs on the inside circles are too short, those circles will fall out during cutting. you need to drag the Vtab across 3 circle segments.

The rectangles at top left are 'backtacking'. they will cut out fine, but slowly, so you will want to fix that.
Remove the cutline.
select the shape
right click and 'phlatten' it
reapply the cuts and tabs.

That usually fixes it, if not, then you need the 'bztools' plugin and use the 'create polyline' function to properly set the directions of all the segments of the outlines.

 

well, in a previous message I did say:

Code:

On circles, use V tabs (press END to swap types) and bridge 3 adjacent arc segments, in 2 or 3 places around the circle, depending on size.This is the only time we place tabs next to each other.

I don't know how to say it more clearly (-: I also attached a file with examples of 3 segments bridged like this, to 'show and tell' as they say.....

 

Gcode has a code to set the units
G20 sets inches
G21 sets millimeters

Read your gcode file to find out what it sent to the controller. (just a text file, read it with notepad)
SketchUcam ALWAYS outputs the units selector, as should every Gcode generator.

Units in Sketchup can be either decimal inches or millimeters and the gcode will be fine.
I don't think any other units like miles has ever been tested (-:

 

Not missing at all. Just choose multipass with a layer depth set to your chosen peck depth.
Then there are new options that control the retract mode, a full retract or a 'quickpeck' small retract.
All detailed in the manual SketchUcam Toolbar

 

in the GRBL settings, halve the max speed and acceleration for X Y and Z. That should get it going reliably. you can tune the values higher later.

 

Do you have the latest version? 1.5a includes the latest version of the gplot.exe program which has improved (but not perfect) panning.
The issue is one of scale, the whole drawing has a scale, the screen has another scale, the current view has yet another scale.
The math to figure out how far a mouse movement relates to the onscreen movement has thus far eluded me. (-:

 

please post your sketchup file and your gcode file here so I can have a close look.

so it has saved just fine at this point, the file exists in the folder you chose with the name you chose..... with extension .nc or .gcode

This is a bit confusing. Gcode files are *just text* so any program that can open a text file can open it, you just have to select 'all files' in the extension selection box of the open file dialog in, for example, Notepad.

OBControl knows about .nc and .gcode extensions (and some others) so will open the file just fine by default, so use the known extensions when you save.

If OBControl is running on the same computer you are using Sketchup on, then click the transfer button (OB logo) in the toolbar to send the gcode (you do have to generate and save it first) into OBControl. (see attached video)


This is only useful if this is the same PC that is controlling the machine, otherwise pretty pointless.

So if your control PC is not the Sketchup PC, it would be normal to

1. save the gcode file
2. transfer the gcode file to the control pc (through the network, or walk over with a flash stick)
3. open OBControl
4. click 'Open G-CODE'
5. select 'Open Gcode from file'
6. select the file
7. click the 'open' button.

A quick video of saving and transferring to OBControl on the same computer is attached. Only useful if your editing PC is also the PC that controls the router.

(for the tech savvy it IS possible to jigger the transfer script to transfer through the network from a 'sketchup pc' to a 'router pc' that is on the same network)

 

oops, missed the attached gcode earlier.

You have somehow infected all your shapes with the backtick disease.

A few posts ago I mentioned that the 2 shapes at top left were a problem and needed to be fixed, and mentioned the tool that does it for you.

What I want to know is what you did after that that has caused every cut to now be backticking?

This is some kind of internal Sketchup thing I think so I need to know what Sketchup version you are using, what license is in effect, what you did in terms of editing, etc etc.
We need to figure it out so that we can prevent or cure it in the future.

Since SketchUcam very rarely has a problem like this with outline cuts this is something new. (was common with centerline cuts)