User Tools

Site Tools


geda:pcb-quick_reference.fr

Autres langues: English 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 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 PCB Manual. Il y a aussi le 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
geda/pcb-quick_reference.fr.txt · Last modified: 2014/04/18 07:37 by vzh