gEDA Project Wiki

This page is read only. You can view the source, but not change it. Ask your administrator if you think this is wrong.
====== PCB: Quick Reference ======

===== Default Key Mapping =====

==== All Keystrokes ====

^  Key		^ Mnemonic	^ Description  ^
|  <key>esc</key>		| select	| enter select mode (same as [space], or [F11])  |
|  esc		| end of action	| terminate the current action, e.g. stop drawing tracks  |
|  insert	| insert point	| enter insert point mode. Click and drag on track to insert a point  |
|  return	| click		| same as a click on the left mouse button  |
|  space	| select	| enter select mode (same as [esc], or [F11])  |
|  tab		| flip up/down 	| view: vertical flip  |
|  shift-tab	| flip left/right 	| view: horizontal flip  |
|  ctrl-shift-tab	| far side	| view: exchange the roles of front side and far side  |
|  del		| delete	| delete object under the mouse cursor |
|  shift-del	| del-sel	| delete objects in selection |
|  backspace	| del-sel	| delete objects in selection |
|  shift-backspace	| del-copper	| deletes connected copper under the cursor. Rats are considered a connection.  |
|  <nowiki>|</nowiki>		| thin-draw	| toggles thin draw mode  |
|  a		| set same	| read the parameters to use for new objects from the object below the cursor.  |
|  alt-a	| select-all	| select all objects on active layers. Deactivated layers are ignored.	|
|  shift-alt-a  | unselect	| clear selection  |
|  b 		| to other side	| flip object to the other side of the board  |
|  c  		| center	| view: center display at cursor position  |
|  ctrl-c  	| copy to buffer| copy selection to buffer and unselect  |
|  d		| display name	| display pin or pad name  |
|  shift-d  	| pinout dialog	| open pinout window for element under mouse cursor  |
|  e		| eliminate rats| delete all rats  |
|  shift-e	| eliminate some rats	| delete selected rats  |
|  f  		| find		| highlight connections to object under mouse cursor. This includes rats and objects on invisible layers  |
|  ctrl-f    | add to found  | add connections to object under mouse cursor to the set of found objects  |
|  shift-f  	| un-find	| un-highlight found connections  |
|  g  		| incr grid mil	| increment grid by configured imperial increment  |
|  shift-g  	| decr grid mil	| decrement grid by configured imperial increment  |
|  ctrl-g  	| incr grid mm	| increment grid by configured metric increment  |
|  ctrl-shift-g	| decr grid mm	| decrement grid by configured metric increment  |
|  h  		| hide		| toggle the visibility of the refdes or value attached to the component under the cursor |
|  shift-h  	| hide sel	| toggle the visibility of the refdes or value attached to selected components  |
|  ctrl-h  	| holeplate	| toggle plating of a via. Used to produce non metalized mounting holes  |
|  j		| lineclear	| toggle the polygon clear flag of the line under the cursor  |
|  shift-j	| lineclear sel	| toggle the polygon clear flag of selected lines  |
|  k  		| klear		| increment clearance (soldermask to copper edge)  |
|  shift-k  	| klear (-)  	| decrement clearance (soldermask to copper edge (NOTE: can go negative!))  |
|  ctrl-k	| klear sel	| increment clearance of selected objects (soldermask to copper edge)  |
|  shift-ctrl-k	| klear sel (-)	| decrement clearance of selected objects (soldermask to copper edge)  |
|  l  		| increase line	| increment width of the line tool, adds to the settings of the current line style  |
|  shift-l  	| decrease line	| reduce the current linewidth |
|  m  		| move to layer	| move the object under the cursor to the current layer  |
|  shift-m  	| move selection to layer	| move selected objects to the current working layer (see [[geda:pcb_tips#how_do_i_move_one_set_of_layer_tracks_to_another_layer|pcb tip]])  |
|  ctrl-m	| move origin	| set the origin to the current position of the mouse pointer |
|  n		| name		| show object refdes / pin number at mouse pointer |
|  shift-n	| next		| Select the shortest unselected rat on the board |
|  o		| optimize rats	| optimize and redraw all rats |
|  shift-o	| optimize some rats	| optimize and redraw selected nets only |
|  ctrl-o	| octagon	| toggle the octagon flag of the object under the cursor  |
|  shift-p	| polygon close	| connect the first point of a polygon with the last  |
|  q		| square toggle	| toggle square/round corners on pads  |
|  shift-r	| redo		| redo what was undone with undo  |
|  ctrl-r	| report	| show object report  |
|  s		| size		| increment size of the object under the cursor  |
|  shift-s	| size (-)	| decrement size of the object under the cursor  |
|  alt-s	| sizehole	| increase the hole of the object under the cursor  |
|  alt-shift-s	| sizehole (-)	| decrease the hole of the object under the cursor  |
|  ctrl-s	| sizehole	| increase the hole of the object under the cursor  |
|  ctrl-shift-s	| sizehole (-)	| decrease the hole size  |
|  t		| text tool size | increase the size of new text by 10 mil  |
|  shift-t	| text tool size (-)| decrease the size of new text by 10 mil  |
|  v		| view extents	| global view of working area  |
|  shift-v	| via tool dia  | increase the diameter of new vias by 5 mil  |
|  ctrl-shift-v	| via tool dia (-)| decrease the diameter of new vias by 5 mil  |
|  alt-v	| via tool drill  | increase the drill diameter of new vias by 5 mil  |
|  alt-shift-v	| via tool drill (-) | decrease the drill diameter of new vias by 5 mil  |
|  z		| zoom		| view: zoom in  |
|  shift-z	| un-zoom	| view: zoom out  |
|  F1		| via		| enter via tool |
|  F2		| line		| enter line tool  |
|  F3		| arc		| enter arc tool |
|  F4		| text		| enter text tool |
|  F5		| rectangle	| enter rectangle tool|
|  F6		| polygon	| enter polygon tool |
|  F7		| buffer	| enter buffer mode | 		
|  F8		| delete	| enter remove mode |
|  F9		| rotate	| enter rotate mode  |
|  F10		| file menu	| file menu |
|  F11		| select	| enter select mode (same as [space], or [esc])  |
|  F12		| lock		| enter lock mode |

==== Viewport Keystrokes ====

^  Key  ^  Mnemonic  ^ Description  ^
|  v		| view extents	| global view of working area  |
|  c		| center	| centers view on cursor  |
|  z		| zoom		| zoom in  |
|  shift-z	| un-zoom	| zoom out  |
|  <nowiki>|</nowiki>	| thin-draw	| toggles thin draw mode  |
|  tab		| flip up/down 	| vertical flip  |
|  shift-tab	| flip left/right 	| horizontal flip  |
|  ctrl-shift-tab	| far side	| exchange the roles of front and far side  |

==== Layers ====
^  Key  ^  Mnemonic  ^ Description  ^
|  1 to 9			| - | select layers 1 to 9  |
|  0				| - | select layer 10 (*)  |
|  alt-1 to alt-9 		| - | select layers 11 to 19 (*)  |
|  alt-0			| - | select layer 20 (*)  |
|  ctrl-1 to ctrl-9		| - | toggle visibility of layers 1 to 9 (*)  |
|  ctrl-0			| - | toggle visibility of layer 10 (*)  |
|  ctrl-alt-1 to ctrl-alt-9 	| - | toggle visibility of 11 to 19 (*)  |
|  ctrl-alt-0			| - | toggle visibility of 20 (*)  |
(*): These accels are available in PCB, GTK GUI in versions after august 2011
====== Footprint Reference ======
The Master document for footprint creation is the [[http://pcb.geda-project.org/manual.html|PCB Manual]]. There is also Stuart Brorson’s [[http://www.brorson.com/gEDA/land_patterns_20050129.pdf|Footprint Creation for the Open-Source Layout Program PCB]].

===== General syntax =====
A pcb footprint file may contain any of the following commands:
  * **''Element [element_flags, description, pcb-name, value, mark_x, mark_y, text_x, text_y, text_direction, text_scale, text_flags]''**
  * **''Pad [x1 y1 x2 y2 thickness clearance mask name pad_number flags]''**
  * **''Pin [x y thickness clearance mask drillholedia name number flags]''**
  * **''ElementArc [x y r1 r2 startangle sweepangle thickness]''**
  * **''ElementLine [x1 y1 x2 y2 thickness] –> thickness != 1000 = 10 mils almost for all footprints''**
  * Comment lines start with the ‘**''#''**’-sign

===== Elements =====
**''Element [element_flags, description, pcb-name, value, mark_x, mark_y, text_x, text_y, text_direction, text_scale, text_flags]''**

^  item  ^  allowed value  ^  explanation  ^  comment  ^
|  element_flags  |  unsigned hex value  |  |  |
|  description  |  string  |  text description of footprint  |written by footprint author  |
|  pcb name  |  string  |  refdes used on this particular pcb  |xxx  |
|  value  |  string  |  value of component on this particular pcb layout  |xxx  |
|  mark_x  |  1/100th mils  |  |  |
|  mark_y  |  1/100th mils  |  |  |
|  text_x  |  1/100th mils  |  |  |
|  text_y  |  1/100th mils  |  |  |
|  text direction  |  decimal integer  |  0=horiz; 1=ccw90; 2=180; 3=cw90  |  |
|  text_scale  |  decimal integer  |  |usu. set 100  |
|  text_flags  |  unsigned hex  |  |  |

===== Pads =====
**''Pad[x1 y1 x2 y2 thickness clearance mask name pad_number flags]''**

^  Item  ^  Allowed Value  ^  Explanation  ^  Comment  ^
|  x1  |  1/100th mil  |  x (1st point)  |   |
|  y1  |  1/100th mil  |  y (1st point)  |   |
|  x2  |  1/100th mil  |  x (2nd point)  |   |
|  y2  |  1/100th mils  |  y (2nd point)  |   |
|  thickness  |  1/100 mils  |  width of metal surrounding line segment  |see Brorson .pdf  |
|  clearance  |  1/100 mils  |  distance to any other copper on any layer  |actually 1/2 of this number is used!  |
|  mask  |  1/100th mils  |  width of mask relief  |actual width of the mask centered on pad copper  |
|  name  |  string  |  name of pad (arb. string)  |e.g. “pad_1” or “positive” or any other string  |
|  pad_number  |  string  |  pad #  | used for nets. it MUST be consistent with the definitions on the netlist.  |
|  flags  |  hex or string  |   | examples:  |

===== Pins =====
**''Pin[x y thickness clearance mask drillholedia name number flags]''**

^  Item  ^ Allowed Value  ^  Explanation  ^  Comment  ^
|  x  |  1/100th mils  |  pin x coord.  |  |
|  y  |  1/100th mils  |  pin y coord.  |  |
|  thickness  |  1/100th mils  |  copper diameter  |  |
|  clearance  |  1/100th mils  |  2*(cu to cu clearance)  |if you want a 10 mil clearance, put 2000 (20 mils) here  |
|  mask  |  1/100th mils  |  diameter of mask aperture  |actual dia. of hole in mask  |
|  drillholedia  |  1/100th mils  |  dia. of hole  |  |
|  name  |  string  |  arb. pin name  |  |
|  number  |  decimal integer  |  pin number used by nets/rats  |  |
|  flags  |  hex  |  xxx  |  |

===== Examples =====
  * **''Pad[-24606 14760 -19538 14760 1181 2000 3181 “” “16” “square”]''**
  * **''Pad[-14760 19538 -14760 24606 1181 2000 3181 “” “17” “square,edge2”]''**
  * **''Pin[0 0 12000 2000 12500 6400 “” “1” 0×00000001]''**
  * **''ElementArc [0 0 6800 6800 0 360 1000]''**
  * **''ElementLine [-26696 -26696 26696 -26696 1000]''**
  * **''# notes within PCB Footprints go after the pound sign''**


====== PCB Command Line Action Reference (abridged) ======
|:FreeRotateBuffer(degrees)||Rotate buffer arbitrarily |
|:MoveObject(x,y,unit) ||Move Absolute (x,y,mil) or Relative(+x,-y,mil)|
|:ChangeClearSize(Selected,<amount>,<unit>)|| Clearance Size|
|:ChangeSize(SelectedPins, SIZE)|| Pin Size |
|:ChangeSize(SelectedLines,+N,mils)|| Line Size |
|:MinClearGap(Selected,<amount>,<unit>)|| Clearance Gap |

  * units can be specified as mm or mil.
  * [[http://pcb.geda-project.org/pcb-20100929/pcb.html#Action-Reference|Action Reference from the PCB Manual]]


====== PCB Physical Layer Reference ======
  * outline layer reference
  * physical layer how-to (outline, direct (x,y) footprint placement, part insertion)
gEDA Project Wiki

User Tools

Site Tools

Page Tools
