Pads Layout

These are my notes as I struggle with using Pads Layout for development of consumer electronics PCB's. Because I sometimes go months between uses of Pads, my notes might be more detailed than necessary for most people, as I tend to forget things.

Be Careful Of ...

  • When using a decal from another person, check the padstack for each pad. Often people neglect to add PasteMask and SolderMask to their padstack.

PCB Finishes -- RoHS / non-RoHS

The main RoHS finish would now be a Lead Free HASL. This is done the exact same way as standard Tin Lead HASL with the exception of it is lead free and comprised of a few more alloys to take the leads place. It works well but occasionally will have a bad solder joint, which is why military and medical are exempt from RoHS.

Other RoHS finishes are Immersion Silver, Immersion Gold, and OSP (organic solder).
Both the Gold and Silver are very flat finishes with Silver being geared more towards high speed RF type designs. Boards with Silver need to be populated a little sooner than other finishes, since they tend to oxidize a little if left unstuffed.

The most common finish when RoHS is not needed is still the Tin Lead HASL. This is also the most cost effective followed by Silver then Gold.

PCB Fabrication Notes

Place Fabrication Notes directly onto your board layout, usually on the drill drawing layer, so that they are available in the gerber files when you create them.

Below are some typical fabrication notes for a six layer board.

    FABRICATION NOTES:
    (USE UNLESS OTHERWISE NOTED)
    
    1) ARTWORK; THIS PCB DESIGN HAS (6) ELECTRICAL LAYERS. FABRICATE BOARD
                USING THIS DRAWING AND THE GERBER PACKAGE 1XX-XXXXPN-00-A.ZIP
                FILES IN THE FOLLOWING STACK-UP: (ALSO SEE DETAIL A)
                *.SST - TOP SIDE SILKSCREEN
                *.SMT - TOP SIDE SOLDERMASK
                *.TOP - TOP SIDE ETCH
                *.GND1 - GROUND PLANE 1 ETCH
                *.PWR - POWER PLANE ETCH
                *.IRT - INTERNAL ROUTE ETCH
                *.GND2 - GROUND PLANE 2 ETCH
                *.BOT - BOTTOM SIDE ETCH
                *.SMB - BOTTOM SIDE SOLDERMASK
                *.SSB - BOTTOM SIDE SILKSCREEN
    
    2) MATERIAL; FR4 GLASS EPOXY N.E.M.A GRADE SUBSTRATE
                MATERIAL (SEE NOTE 12) SHALL MEET UL FLAMMABILITY
                CLASSIFICATION 91-V1 OR BETTER
    
    3) COPPER THICKNESS; ALL LAYERS TO BE 1.0 OZ. FINISHED WEIGHT
    
    4) FINISHED BOARD THICKNESS: 0.062" +/-0.007"
    
    5) BOARD CONSTRUCTION; L.P.I SOLDERMASK OVER BARE COPPER.
    
    6) FINISH; COPPER PLATE ALL HOLES TO A MINIMUM 0.001" THICKNESS.
               PLATING SURFACE FINISH SHALL BE ELECTROLESS NICKEL/IMMERSION GOLD
               PER STANDARD IPC-4552 (SEE NOTE 12)
    
    7) APPLY SILKSCREEN NOMENCLATURE USING WHITE EPOXY INK.
    
    8) FINISHED HOLE DIAMETER TOLERANCE; +/-0.003"
    
    9) ALL BOARD DIMENSION TOLERANCES; +/- 0.005"
    
    10) BOARD FABRICATION PROCESS MUST BE UL APPROVED.
    
    11) ALL VENDOR MARKINGS TO BE IN INK OR MASK NOT TO ALTER THE COPPER
    
    12) BOARD SHALL BE EU RoHS COMPLIANT

Generate Gerber Files

After your layout is done, you need to create a set of gerber files that you can send to a pcb board house. I like Quick Turn Circuits for good quality, quick, cheap PCB's.

  • Load the PCB Layout into Pads Layout
  • Repour your copper pours, as they do not save
    • Select Tools - Pour Manager - Flood All - Start
  • Select File - CAM
  • Select all your layers, down to the N/C-Drill layer
  • Click Preview Button to see each layer to make sure there are no problems
  • Click Run Button
  • Add a contact.txt file to the pile of gerbers, with your name, email and phone number
  • Zip all the gerbers up into a zip file, and email them to your pcb house for fabrication

Centroid File - ASCII CAD data

Some board stuff houses like to use what they call a centroid file to help them program their pick and place machine. Generally, they will accept an ascii export of your pads layout file.

  • Load the PCB Layout into Pads Layout
  • Select File - Export
    • The ASCII Output dialog box opens
  • Select all sections by clicking Select All
    • If the part type library contains attributes, select Include LibAttributes
  • Select PADS Layout V2007
  • Click OK
  • This will generate a file with a .asc extension.
  • I like to throw this into the same pile as my gerber files and zip them all up together.

Create Library from a Layout

If you have an existing layout with components on it, and you wish to create a library file with these components.

  • Create a new library to put them in
    • Open the Library Manager
      • Menu - File - Library
    • Click 'Create New Lib.'
    • Select where you want your new library to be, name it, and create it
    • Close the Library Manager
  • Click on an empty area of your layout to deselect any active mode
  • Right click on empty area of your layout to bring up Menu
  • Click 'Select Components'
  • Right click on empty area of your layout to bring up Menu
  • Click 'Select All' (or hit CTRL-A)
    • Now all your components in the existing layout have been selected
  • Right click on empty area of your layout to bring up Menu
  • Click 'Save to library'
  • Select the new library you just created
  • Done - You now have a library with all your components which you can use in other designs.

Update a decal in the library

After you've modified a decal on your board, you may want to update your library.

  • Click 'Select Components'
  • Click on the component you want to save to the library
  • Right click on empty area of your layout to bring up Menu
  • Click 'Save to library'
  • Select the library you want to save to
  • Done - You have saved your component changes back to the library

Refresh the PADS layout after a change in the decal library

If you want your decal changes to show up in your current layout after the decal is changed in the library.

  • Highlight the part on the board
  • Go to ECO Toolbar
  • Select Change Component button
  • Select Library Browse
    • Right click somewhere on your design to bring up this menu
  • Check the Box; Update Part Type from Library
  • Under Part Types Highlight the Part Type and
  • Click Replace
  • Finally, save your revised PCB layout to file.