I’ve been very busy since the start of the year and haven’t managed to post anything new. There will be some posts coming up now though. I received some new PCBs today, will post some pictures and info soon. Also I will be making a post about the stuff that I’ve been working on for the past few months. But more about that when I find some time. Will be awesome, I promise you that.

But now, to the topic on hand. Many people don’t usually use hotkeys, macros, commands etc in the programs they use. Most of the time I don’t either, but given that I use EagleCAD alot, I decided to optimize my workflow. I started out with using the command line input, but after some time it felt kind of slow, so I also made some hotkeys and macros to improve my workflow even further. I have to admit, I was quite surprised how much faster I got my work done. So here is a short overview how I managed that.

Commands I use frequently:
Schematic editor
gr on //displays grid
a //opens component adding menu
v //add value to the component
fr //draw frame
sm //smash
pack //displays the alternative packages menu
er //ERC test
tex //add text

Board editor
gr on //(grid on) displays grid
gr mm //change the grid units to mm
gr a mm //change alternative grid units to mm
gr .2 //change grid size to 0.2 mm
gr a .05 //change alternative grid size to 0.05 mm
pack //displays the alternative packages menu
dr //DRC test
po //polygon tool
c w .3 //change trace width 0.3
c w .2;vi //changes via drill to 0.2 and selects via tool
c is .3 //changes isolation to 0.3
c sto on //changes stop on

And some minimized displaying commands for most used layers
di none //clears all
di v //display Via
di p //display Pads
di u //display Unrouted
di d //display Dimension
di t //display Top
di b //display Bottom
di tor //display tOrigin
di bor //display bOrigin
di td //display tDocu
di bd //display bDocu
di tp //display tPlace
di bp //display bPlace

Useful in both
sh c* //shows everything that starts with the letter c, mostly capacitors. sh r* can be used to show the resistors for example. I suggest you read more about the wildcards in the Eagle manual, very useful stuff
sh @ c23 //shows and draws a box around the C23 capacitor

If you are using the route tool for example, you can change the width of trace by just writing “.3” and it changes the width to 0.3mm, very useful and fast

Hotkeys and macros I use constantly (they can be set under Assign menu):
Schematic editor
Ctrl + Q > move
Ctrl + W > net
Ctrl + E > group
Ctrl + R > show
Ctrl + A > copy
Ctrl + D > delete
Ctrl + F > info
Ctrl + T > name
Ctrl + G > label

Board editor
Ctrl + Q > move
Ctrl + W > route
Ctrl + E > group
Ctrl + R > show
Ctrl + A > copy
Ctrl + D > rip
Ctrl + F > info

F1 > set POLYGON_RATSNEST OFF; rat; SET POLYGON_RATSNEST ON //only calculates the airwires, won’t recalculate the polygons, alot faster on boards with lots of components
F2 > rat

Ctrl + 1 > disp none unrouted dimension vias pads top bottom tplace bplace torigin borigin tdocu bdocu
Ctrl + 2 > disp none unrouted dimension vias pads top tplace torigin tdocu
Ctrl + 3 > disp none unrouted dimension vias pads bottom bplace borigin bdocu
Ctrl + 5 > disp none dimension unrouted vias pads top
Ctrl + 6 > disp none dimension unrouted vias pads bottom

Some useful ULPs
run bom //generates bill of materials

run statistic-brd //lots of stats about the board
run length //calculates the trace lengths
run count //counts drills, pads, vias etc

If you find any mistakes or have some further suggestions, feel free to contact me.