Protel 99 SE

• the choice between the slow database and a fast file approach to
  store the files. The database approach uses a crappy database,
  so I prefer the files.
• an outputfile manager. In the previous version you had to look at
  many different places until you had the gerber files and the drill files
  together.

My tips

Printouts for 'etch-your-own' pcb

• Add a new printout named 'toplayer'
• Add a new layer : multilayer
• Move the multilayer to the top
• Select 'showholes', 'black&white', 'mirror layer'
• Add a new printout named 'bottomlayer'
• Add a new layer : bottomlayer
• Add a new layer : multilayer
• Remove the toplayer
• move the multilayer to the top
• select 'showholes', 'black&white'

Now print the two new printouts to ester foils
.There is also a yahoo group concerned with making your own pcb. Homebrew_BCBs

Unhide hidden items in schematic editor

1. double-click on the component.
2. check the "view hidden fields" radio button
3. exit view (OK)
4. double-click on the item of interest
5. check the appropriate view radio button
6. exit view (OK)
7. double-click on the component
8. un-check the "view hidden fields" button
9. exit view (OK)

1. place a new component
2. copy the identifier
3. copy the value or set a new
4. delete the old

A bigger job : recovering the pcb from gerber

• the latest Gerber data from an email sent to the manufacturer
• the latest schematic on paper
• the schematic file a week old
• the pcb file also a week old

1. make a new project, copy schematic
2. update the schematic manually to the latest version
3. new pcb, open this pcb
4. from the files menu : import, filetype = gerber batch, select ...
   the layout, without the vias, without the nets, without the parts
   is here now
5. remove the power plane :
   select GND : Edit/Select Connected Copper, Sel=GND,
   delete GND : Ctrl Del, and it is gone, or perhaps just a part of it.
   
6. get the components :
   In the schematic : Design/Update PCB
   
7. place the components :
   snap = 1mil, disable online DRC, disable electrical snap
   starting with the complex parts, eg cpu, connectors, place them
   were they were. It goes rather quick as the connections are shown
   with lines.
8. get the nets, place the vias :
   Design/Netlist Manager/Menu../Update Free Primitives from Component Pads
   assigns the net to the tracks. The vias can be placed on assigned tracks
   and they then get the net from the track. Repeat that until all vias are
   placed and all tracks are assigned a net.
9. Get the GND plane :
   Setup the Design/Rules as they were : width, gaps and so on
   Pour the GND poly

While that (page) does describe a process for recovering a file from gerber, 
it does not give the most efficient way of doing so.

The process I would use is to start with free track and pads brought in 
from gerber. (vias are plotted the same as pads, so they import as free 
pads.) Save that file separately. I would then place the footprints so that 
the pads overlay exactly. It is also possible to recreate a footprint by 
copying the pads (through the clipboard) into a footprint (in the library 
editor). Then I would delete all free track and pads. I would then import 
the net list or run Update from the Schematic. Then I would open the 
separate file with track and pads. I would use global edits to delete all 
footprint pads, typically they would be different sizes from vias or free 
pads. When I have the file with only track and free pads, I would use Tools 
Convert to change all the free pads to vias (or those which are 
appropriate, if there are other free pads on the board). I would then copy 
this en masse to the PCB with the footprints. It will help if the block 
copy reference is in the same location as a footprint pad. When a block is 
copied, the default is that copied track and vias and pads pick up the net 
from already-existing primitives....

I haven't tested this recently; if the net assignments are not complete, 
the Update Free Primitives process should complete it.