Protel 99 SE

December 99, I received the free upgrade to the protel 99 SE
Beside introducing a few bugs, perhaps intended as new feature,
the noteworthy changes are :

My tips

Printouts for 'etch-your-own' pcb

In the pcb view select 'files, print/preview. Then in the 'browse pcbprint':

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

It can happen that one did hide a field 'RES1' instead of assigning a value to it.
The reverse is rather unelegant. there are two choices :
The hard way :
  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)
The simpler way :
  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

Due to a disk crash I lost about a weeks work. I had : The biggest work of this lost week was the manual routing, required for the highfrequency operation at 200MHz. The recovery was done as :
  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
It took me 2 days.

A comment on my previous explanations from Mr Abd ulRahman Lomax :

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.
I haven't tested it either, as I'm happy to have recovered it at all, but perhaps next time ...


last updated: 4.may.02

Copyright (99,2001) Ing.Büro R.Tschaggelar