Text in Copper Zone


#21

I pushed this update to github. My impression is that uptake on KiCommand is fairly low at the moment, so there may very well be bugs that slip by.

I’ve added a core command topoints and modified todrawsegments to accept point pairs in addition to tracks. Given this, I had to do some cartwheels to get the width from the text and apply them to the drawsegments. Those cartwheels are documented in the texttosegments command.

Usage: toptextobj selected Dwgs.User texttosegments F.Cu tocopper

The first two commands retreive all the selected top text objects. Then Dwgs.User texttosegments copies the text objects to the Dwgs.User layer, then the F.Cu tocopper copies those segments to the F.Cu copper layer.

Let me know if you have any problems or questions!

Here is the definition of texttosegments in the persist file (which you never have to look at):

:persist texttosegments "Draw [TEXTOBJLIST LAYER] Copies text objects in TEXTOBJLIST to LAYER."
        swap copy GetThickness call list swap 
        topoints pairwise 2 pick todrawsegments 
        copy 2 pick SetWidth callargs pop
        swap pop swap pop
        ;

#22

I’ve been watching your progress on KiCommand since you started. I’ve yet to understand a task that it does that I might want to do; and to spend the time to learn it.

If KiCommand can draw text on copper as per the OP then I can clearly see the issue and that KiCommand is the solution.

Can KiCommand help design really complex edge cuts?


#23

I think so. I’ve been trying to add useful geometry commands that assist with drawsegments and arcs into polygons.

Here is a list of interesting Draw and Geometry commands that might help:
Draw - drawparams outlinepads drawarctest outlinetoptext param newnet texttosegments orthogonal showparam grid findnet round pad2draw makeangle scale drawarc topoints outlinetext drawtext drawsegments cut regular

Geometry - rotatepoints areacorners rotate corners angle topoints ends wxpoint setlength length

One thing that might help is for you to define a specific complex edge cut, then I can see if the commands exist to create it. And if not, I might be able to create new commands that would help.

P.S. My comment on “uptake…fairly low” was not a specific complaint at all, just a reason that updates may include bugs at this point. I haven’t yet implemented any type of automated testing. And I totally understand that people will try it out when they have time and a specific need that KiCommand seems to solve.


#24

I don’t know if you will believe me…

I want to create a pcb that looks like a one eyed one horned flying purple people eater.

Less complex, but similar, to this:


#25

Can you define each vertex as an x,y point? if so, then you can use drawsegments:

drawsegments (Category: Draw) 
	[POINTSLIST] Points list is interpreted as pairs of X/Y
	values. Line segments aredrawn between all successive pairs
	of points, creating a connected sequence of lines where each
	point is a vertex in a polygon as opposed to being just a
	list of line segments or point pairs. This command uses
	previously set drawparams and the points are in native units
	(nm) so using mm or mils commands is suggested. 

Or you could define the body, one arm, one ear and one leg, then copy and rotate as appropriate, using rotate and/or makeangle. I think you can also program move commands.

That does make me think of a new command, perhaps outline that will traverse the outline considering the indicated drawsegments as merged polygons.

Does any of this sound interesting for your problem?


#26

You do realize that if you can do this, then not having to use a Cad or Drawing program to export and import would be a pretty cool thing to document how to do.


#27

drawsegments is easy.

First define the param, which are the default layer, thickness and other draw parameters.

Then list the points you want connected with line segments. Just a list of x then y repeated as many times as you need:

0.3 mm t param Edge.Cuts l param
0,0,10,0,10,-10,0,-10,0,0 mm drawsegments

There’s an error in drawsegments that currently misinterprets the layer, so it must be entered like this:

0.3 mm t param Edge.Cuts layernums l param

But I’ll fix that next release.

You can also select whatever you’ve drawn and scale all segments selected to any desired dimension.

Edit to add: and when you’re done, you can round each vertex to a specific radius.

round (Category: Draw) 
	[RADIUS SEGMENTLIST] Round the corners of connected line
	segments within SEGMENTLIST by adding ARCs of specified
	RADIUS.

#28

I’m still not used to using KiCommand.
Where is the command prompt? I tested some examples from the README and your new function… but non of them works.


#29

Another example

On Windows 10 with KiCad 4.0.7 I cannot use KiCommand…
May I upgrade to the nightly build?


#30

I would stick with 4.0.7 as that is what I am testing on (Windows 7).

The toptextobj… command string may fail with that message if you don’t have any text selected.

The others were basic coding errors on my part that I hadn’t tested in a long time.

I’ve pushed a new version of KiCommand to github that fixes the other errors you mention.


#31

Also note that the load command which is usually used to load user commands can actually be used to read in any commands. So you could put a large number of drawsegments commands as above into a file and load them to create a sequence of lines on your board.

Edit to add: if you let the param values be defined externally before loading the file, you can use the drawsegments to draw on any non-copper layer.


#32

I went online and found coordinates to plot, translated it into an input file

2,12,2,13,3,14,5,15,5,13,2,12,0,11,-3,8,-4,10,-3,10,-4,13,-3,13,-2,15,-1,15,1,17,1,16,2,17,4,18,5,18,7,19,7,18,9,19,11,19,10,18,11,17,11,16,12,14,10,14,10,13,8,13,7,12,7,9,9,9,9,10,8,11,7,11 mm drawsegments
-1,10,0,8,-2,7,-2,4,-1,3,1,5,3,6,4,6,5,5,6,6,7,5,8,5,10,6,10,7,9,8,7,9 mm drawsegments
9,19,7,21,4,22,-4,20,-7,18,-8,15,-8,13,-7,11 mm drawsegments
10,7,11,8,12,7,13,7,14,9 mm drawsegments
10,14,8,15,7,15,7,14,5,13 mm drawsegments
7,14,9,13,10,12,9,9 mm drawsegments
10,13,11,11,13,10,15,8,18,6,19,2,18,-1,18,-3,16,-7,12,-12,9,-12,5,-11,2,-10,-1,-8,-4,-7,-6,-3,-7,-2,-9,-2,-10,-3,-11,-5,-11,-6,-10,-7,-8,-8,-6,-7,-5,-5 mm drawsegments
15,8,15,5,14,4,10,2,8,0,7,0,6,1,4,1,2,0,-1,1,-3,3 mm drawsegments
-3,8,-3,3,-6,-3 mm drawsegments
-8,13,-10,8,-10,5,-8,0,-8,-2 mm drawsegments
5,8,6,11,5,12,4,12,3,11,3,8,5,8,5,9,4,10,3,10 mm drawsegments
6,1,9,4,8,3,10,2 mm drawsegments

Placed the file into: ~/kicad/kicommand/drawing.txt

Then went into kicommand and drawing.txt load.
Then selected the drawing and drawings selected 180 rotate

And ended up with:


(The red lines are the default frame because the coordinates in the drawing file overlap the frame lines).

This works in OpenGL canvas and 4.0.7 still requires to switch canvases after drawing with kicommand or python to see the new line segments (use F9 then F11).


KiCommand released on github - Easy pcbnew command strings; 4.07 & nightly
#33

I created an update and added a few commands, including fromsvg that can take the ‘d’ attribute from the ‘path’ element of an SVG file.

I took the graphic and traced over it with straight lines in inkscape then took the resulting SVG:

Then I created the following command in KiCommand (it’s quite a long string and must be on one line within double quotation marks):

"m 81.38357,74.230848 5.612659,1.870887 5.211757,3.474503 2.138156,2.138157 10.958048,-6.1472 0.53454,5.078121 -1.06908,4.009044 -2.80633,4.276312 -2.539056,1.603616 1.202716,4.276312 9.48806,-2.939963 13.36348,8.686253 -8.95353,-0.4009 -2.13815,5.34539 -5.21176,-2.67269 -4.67722,4.54358 -2.40542,-3.0736 -4.009046,6.94901 -3.741775,4.27631 -4.142676,2.53906 1.870887,3.34087 v 3.34087 l -4.409948,2.53906 h -2.806329 l -2.80633,-0.53454 -0.267271,-2.00452 1.469982,-1.60362 0.668176,-0.4009 -0.53454,-1.73726 -4.142676,0.53454 -4.677217,-0.93544 -3.34087,-0.66817 -1.336347,-0.13364 -2.405428,3.87541 -1.469982,1.33635 -1.603616,0.66817 -5.479026,-0.66817 -2.405425,-2.80633 -0.133636,-1.60362 3.207235,-3.34087 1.870887,-2.53906 -2.80633,-2.93996 -2.672696,-4.40995 -0.668174,-2.40543 -4.409945,5.47903 -3.207234,-5.34539 -5.078121,2.13815 -3.474506,-6.14719 -8.285356,0.26726 13.229844,-8.418985 10.022607,4.81085 0.400905,-5.34539 -3.741775,-2.138156 -2.405425,-3.474503 -0.668173,-3.073601 v -7.884451 l 13.363474,5.078121 3.608139,-2.939965 5.211757,-2.271789 3.875408,-1.33635 2.138156,0.133636 3.207234,-3.474503 4.677217,-2.939965 2.405425,-0.668174 z" 1 mm fromsvg drawsegments

This results in the following within KiCad:

With preceding param command to set the layer and the thickness, it can be drawn on any non-copper layer (including Edge.Cuts). Then if followed by the tocopper command, it can be put on any copper layer.

Is this what you had in mind?


KiCommand released on github - Easy pcbnew command strings; 4.07 & nightly
#34

That is pretty cool!
I just have not had the time to spend on this.
Any chance you can export that something I can easily use?


#35

Not sure what you mean. If you install KiCad and cut/paste the command I listed into the KiCommand dialog box, it will draw the line segments just like I pictured.

What else did you have in mind?


#36

I need to figure out how to run KiCommand.


#37

Link to installation instructions, just copy some files:

If you’re running 4.0.7, bring up Script Console and type: import kicommand


#38

I’m trying to used KiCommand to render the selected text object on the F.Cu layer. Using current github master and the following command:

toptextobj selected Dwgs.User texttosegments F.Cu tocopper

I’m seeing activity on the KiCommand stack as presumably operations are executed, but I don’t see either the segments show up on Dwgs.User or the final result on F.Cu. Any ideas, @HiGreg?


#39

Try changing the view to legacy and back to OpenGL. This should refresh the display so you can see the new objects.


#40

That was it! After refilling my ground plane, it looks great. Thanks for making this so easy with KiCommand.