//Autres langues: [[pcb-quick_reference|English]] [[pcb-quick_reference.ru|РуÑÑкий]]//
====== 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†“squareâ€]''**
* **''Pad[-14760 19538 -14760 24606 1181 2000 3181 “†“17†“square,edge2â€]''**
* **''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''**