Index: pnp-origin/index.html
===================================================================
--- pnp-origin/index.html (nonexistent)
+++ pnp-origin/index.html (revision 9571)
@@ -0,0 +1,119 @@
+
+
+
+ pcb-rnd - license
+
+
+
+ pick and place - origin
+
+ A. simplest case: recangular board, implicit outline, implicit P&P origin
+
+Assume a board of 775*725 mils needs to be
+created. The P&P fab says coord 0;0 is the lower left corner. The board
+fab says they need the centerline of toolpath on the outlnie layer for
+milling.
+
+By far the simplest way to handle this board is to rely on builtin defaults:
+
+ - board size (width and height) specifies the outline of a rectangular board
+
- if the outline layer exists but is empty, an implicit rectangular outline is drawn, matching board sizes
+
- implicit P&P origin is the lower left corner
+
+
+Setting it up:
+
+ - 1. start pcb-rnd with no board - this gets the default board template
+
- 2. change board width & height (gtk: file/preferences/user PoV/sizes)
+
- 3. do the layout
+
- 4. when exporting gerber, enable the 'all layers' option to get the implicit outline layer
+
- 5. export the xy
+
+
+
+
+| Pros | Cons
+ |
|---|
+
+ - easy to set up
+
- no need to draw the outline
+
+ |
+ - limited drawing area - unsuitable for editing small boards
+
- supports rectangular shapes only
+
+ |
+
+ B. recangular board, explicit outline, explicit P&P origin
+
+Assume another board of 775*725 mils needs to
+be created. The P&P fab says coord 0;0 is the lower left corner. The
+board fab says they need the centerline of toolpath on the outlnie layer
+for milling.
+
+This time the virtual board (canvas, drawing area) will be larger and the
+board outline of a 775*725 will be manually drawn. Since pcb-rnd won't make
+a guess of where the lower-left corner is, an explicit origin mark
+needs to be added for the pick&place process.
+Setting it up, assuming the GTK HID:
+
+ - 1. start pcb-rnd with no board - this gets the default board template
+
- 2. draw the 775*725 mils box on the outline layer anywhere in the drawing area
+
- 3. do the layout within this box
+
- 4. draw a short line on a random layer - this will be the P&P mark
+
- 5. drag&drop move the endpoint of the unselected mark line to its other endpoint - this will result in a 0 long line, which looks like a filled circle; with 's' increase the size so that it's easily visible
+
- 6. select the mark, drag&drop move it to the lower left corner of the outline box
+
- 7. the mark still selected, press ctrl+e and click on the "add attribue" button in the property editor
+
- 8. type in "pnp-origin" in the "Attribute key" and "yes" in the "Attribute value" field; click ok and close the property editor
+
- 9. export the gerber and xy files
+
+
+There is a video tutorial available on steps 4..8.
+
+Note 1: the mark is not explicitly visible in the XY file. It is not explicitly
+passed to the P&P fab. Instead, all element coordinates are calculated considering
+the mark's center as 0;0.
+
+Note 2: still, the mark is not hidden or suppressed by pcb-rnd from any
+of the output. It must be a line, but it can be on any of the layers.
+Thus the mark potentially would show up on the board. There are multiple
+options to make the mark disappear:
+
+ - make the mark diameter smaller that the router mill bit diameter and place
+ the mark on a copper layer; the board fab will have the copper dot, but it
+ will be milled away.
+
- same trick should work with silk as well
+
- or even on the solder mask layer where this object would be a small cutout over void
+
- make a new (copper) layer, place the mark there and don't send this layer's gerber export
+ (later on pcb-rnd will support documentation layers which are more dedicated for this sort of use)
+
+
+
+| Pros | Cons
+ |
|---|
+
+ - drawing area (canvas) is bigger than the board: easier to edit
+
- can handle slots, cut-outs on the outline layer
+
- if the pick and place fab requires a slight offset on the placement, it is easy to move the mark
+
+ |
+ - requires more steps to set up
+
+ |
+
+ C. round board, explicit outline, explicit P&P origin
+
+Assume a third board shaped as a 700 mil
+diameter circle. The P&P fab says coord 0;0 is the lower left corner of
+the bounding box of the circle. The board fab says they need the
+centerline of toolpath on the outlnie layer for milling.
+
+The process is the same as in example A. The only extra consideration
+is how to find the coords of the P&P origin mark; for this the P&P fab
+house needs to be consulted.
+
+There is a video tutorial available on using temporary
+lines to aid placing the mark for a round lower-left corner.
+
+
+