Just wondering what is the best software to use … a general idea of what steps to take … and any gotchas I need to look out for.
Thanks for any help.
With regards to "best" software. This will be heavily dictated by price. Name your budget. $0, $500, $1000, or $10k.
Two main pieces in the software package:
1. Schematic capture software
2. PCB layout software
Steps:
1. Make schematic symbols with capture software.
2. Make padstacks (the PCB pads for the physical component).
3. Make the footprint of the component using the PCB pads for use in the PCB layout.
4. Make schematic and label schematic symbols with their associated footprint file.
5. Generate a netlist from the schematic.
6. Import the net list into PCB layout software
7. Lay out the PCB.
8. Generate the gerber files, drill files, and if automated assembly, the pick-and-place files, solder stencil, bill of materials, etc.
9. Open up the gerbers in Gerber software (you can find free ones to use. I use "DFM Now!") to view the physical copper layers, silkscreens, and outlines of the board as they will be manufactured and make sure everything looks right. (
You must do this step! PCB layout has a lot of configuration options that can be missed so you must always look at the physical file after it is generated to make sure you didn't mess something up. Seeing the clean layers separately also helps you spot errors that you would otherwise miss in the PCB layout software which can be very crowded even if you turn some layers off since certain things from other layers can still have limited visibility).
10. Send off to PCB fab
11. Hope you made no errors.
Gotchas? Ummmm...
1. Solder masks should be a little bit larger than the copper pad due to tolerances (0.1mm or 4mils larger on each side seems to be standard)
2. Solder paste masks (for automated assembly) should typically be a bit smaller than the copper pad. 0.1mm or 4mils smaller on each side is standard.
3. But some people just use the same size for the copper pad, solder mask, and solder paste mask
4. Be aware that heavy copper boards can't have traces that are as fine or as closely spaced together as lighter copper boards.
5. Ground and voltage planes make routing much easier since those connections go everywhere and without those planes, it's an artform to get those connections jumping over every other trace to get them to go where you want.
6. 0.3mm seems to be the standard minimum via size before you have to jump to start using more specialized processes
7. Make sure your all your net names for ground and other voltages are generated properly in the netlist and PCB layout. I've heard of buggy schematic capture software (big names) that sometimes generate multiple ground net names in the netlist. (e.g. instead of "GND" for eveyrthing, some are "GND", some are "GND_0129938", others are "GND_28375739", etc.)
8. Via stitching is cool
9. Make sure your vias connect to the plane they are supposed to connect to I know that at least PCB layout in OrCAD has a peculiar way of handling the net that a via is connected to (vias don't necessarily retain their net when copied and place onto another plane, they either take the net of the new plane or lose their net altogether and become isolated) and you can't just click on a via and arbitrarily change it's net. The net must be added onto the plane it is intended for and never be moved off that plane.
10. Make sure your PCB silkscreen designtations for components don't get covered up by pads...this was not obvious to me even when examinig the Gerbers. It only became obvious after I received the PCBs.
11. Always check the footprints files made by someone else against at least one datasheet for a component you are using of the same package. I've even had times where the footprint data on the datasheet was incorrect.
12. You can print the PCB out 1:1 on paper and test it against real components before you send the PCB off.
13. Don't have unconnected sections of copper on your PCB. (e.g. a section of copper plane on an outside layer has become disconnected from everything else by traces surrounding it. Either remove it using the function in the PCB layout software or put a via in it to connect it to an internal plane. Or else it can act like an antenna.
Do you need basic electrical design pointers like:
1. placing decoupling capacitors (0.1uF of ceramic X5R or X7R type if you don't know any better) as close as possible to the power pins of all ICs?
2. Keep traces to ground and power planes as short as you can.
3. PCB planes, grounding, and plane partitioning. Really good stuff:
http://www.hottconsultants.com/tips.html
The most important stuff IMO, are the following sections:
It would really help if we knew what kind of PCB it was since that would narrow down pointers a lot.