//Autres langues: [[pcb-quick_reference|English]] [[pcb-quick_reference.ru|Русский]]//
====== PCB: Référence Rapide ======

===== Disposition des Touches =====

==== Table des Touches PCB ====

^  TOUCHE	^ MNEMONIQUE	^  DESCRIPTION  ^
|  esc		| panner	| enter panning mode |
|  insert	| insert point	| enter insert point mode. Click and drag on track to insert a point |
|  space	| select	| entrez en mode select  |
|  tab		| flip view	| view: flip board  |
|  shift-del	| del-cu	| deletes electrically connected copper (including power and signal planes)  |
|  \		| thin-draw	| toggles thin draw mode  |
|  shift-alt-a  | unselect	| clear selection  |
|  b 		| to other side	| flip object to the other side of the board  |
|  shift-b  	| flip view	| view: flip board  |
|  c  		| center	| view: center display at cursor position  |
|  ctrl-c  	| copy to buffer| copie la sélection vers le tampon et désélectionne  |
|  d		| display name	| affiche le nom de la broche ou pastille  |
|  shift-d  	| pinout dialog	| open pinout window for element under mouse cursor  |
|  e		| eliminate rats| efface tous les rats  |
|  shift-e	| eliminate some rats	| efface tous les rats sélectionnés  |
|  f  		| find		| highlight connections to object under mouse cursor  |
|  shift-f  	| un-find	| un-highlight found connections  |
|  g  		| increase grid	| increment grid by configured grid increment  |
|  shift-g  	| decrease grid	| decrement grid by configured grid increment  |
|  h  		| hide		| toggle the visiblity of the refdes or value attached to the current component  |
|  ctrl-h  	| holeplate	| toggle plating of a via. Used to produce non metalized mounting holes  |
|  k  		| klearance	| increment clearance (soldermask to copper edge)  |
|  shift-k  	| klear (-)  	| decrement clearance (soldermask to copper edge (NOTE: can go negative!))  |
|  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 |
|  shift-p	| polygon close	| connect the first point of a polygon with the last  |
|  q		| square toggle	| toggle square/round corners on pads  |
|  ctrl-r	| report	| show object report  |
|  s		| size		| augmente la taille  |
|  shift-s	| size (-)	| diminue la taille  |
|  alt-s	| sizehole	| augmente la taille du trou  |
|  alt-shift-s	| sizehole (-)	| diminue la taille du trou  |
|  ctrl-s	| sizehole	| augmente la taille du trou  |
|  ctrl-shift-s	| sizehole (-)	| diminue la taille du trou  |
|  v		| view extents	| vue globale de la zone de travail  |
|  z		| zoom		| voir: agrandir  |
|  shift-z	| un-zoom	| voir: réduire  |
|  F1		| via		| entrer l'outil de via |
|  F2		| line		| entrer l'outil de ligne  |
|  F3		| arc		| entrer l'outil d'arc |
|  F4		| text		| entrer l'outil de texte |
|  F5		| rectangle	| entrer l'outil de rectangle  |
|  F6		| polygon	| entrer l'outil de polygone  |
|  F7		| buffer	| entrer l'outil de mode tampon |
|  F8		| delete	| entrer l'outil de mode supression  |
|  F9		| rotate	| entrer l'outil de mode de rotation  |
|  F10		| file menu	| menu fichier  |
|  F11		| select	| entrer dans le mode sélection (comme [space])  |
|  F12		| lock		| entrer dans le mode lock |

===== Touches de Visualisation =====

^  TOUCHE  ^  MNEMONIC  ^  DESCRIPTION  ^
|  esc  |  panner  |  |
|  v  |  view extents  |vue globale de la zone de travail|
|  c  |  center  |centre la vue sur le curseur|
|  z  |  zoom  |agrandissement|
|  shift-z  |  un-zoom  |  |
|  \  |  thin-draw on/off  |toggles thin draw mode|
|  tab  |  flip view  |retournement carte|
|  shift-b  |  flip view  |retournement carte|

====== Référence d'Empreintes ======

Le document maître pour la création d'empreintes est le [[http://pcb.geda-project.org/index.html#dir|PCB Manual]]. Il y a aussi le [[http://www.brorson.com/gEDA/land_patterns_20050129.pdf|Footprint Creation for the Open-Source Layout Program PCB]] de Stuart Brorson.

===== Syntaxe Générale =====

Un fichier d'empreinte pcb peut contenir une des commandes suivantes:
  * **''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''**
  * Les lignes de commentaires débutent avec le signe ‘**''#''**’

===== Éléments =====
**''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 descriptif de l'empreinte  |écrit par l'auteur de l'empreinte  |
|  pcb name  |  string  |  refdes utilisé pour ce pcb particulier  |xxx  |
|  value  |  string  |  valeur du composant sur ce pcb particulier  |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  |  |  |

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

^  Item  ^  Allowed Value  ^  Explanation  ^  Comment  ^
|  x1  |  1/100th mils  |  x(1st point)  |  |
|  y1  |  1/100th mils  |  y(1st point)  |  |
|  x2  |  1/100th mils  |  x(2nd point)  |  |
|  y2  |  1/100th mils  |  y(2nd point)  |  |
|  thickness  |  1/100 mils  |  épaisseur de métal entourant le segment de ligne  |voir le .pdf de Brorson  |
|  clearance  |  1/100 mils  |  distance vis à vis des autres zones de cuivre sur toutes les couches  |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 value  |  xxx  |  |

===== Broches =====
**''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  |  |

===== Exemples =====
  * **''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''**
