Author Topic: What are the top "traps for young players" in basic PCB design?  (Read 5601 times)

0 Members and 1 Guest are viewing this topic.

Offline jolshefsky

  • Regular Contributor
  • *
  • Posts: 227
  • Country: us
    • Jason DoesItAll
Re: What are the top "traps for young players" in basic PCB design?
« Reply #25 on: May 02, 2016, 07:19:24 pm »
Here's some hints from Sparkfun on their designs (from 2008). I could swear they posted a checklist at one point (e.g. things to check prior to making a board) but I couldn't find it but I had made my own based on it:
  • Confirm ERC on schematic.
  • Print schematic and review.
  • Silkscreen board name, version, date, creator, company.
  • Silkscreen version information from CVS.
  • Check size of PCB edges against specification.
  • Check for unconnected nets.
  • Confirm DRC on board.
  • Check Gerbers in local software.
  • Print board at 100% size.

I think a general rule that covers a lot of what has been suggested is, "don't rely on someone else's work until you understand how to do it yourself." Footprints are a big example: in both Eagle and now KiCAD I started out trying to use their footprints, but after having problems I now always make my own for each part based on the diagram in the datasheet and the suggested landing pattern.
May your deeds return to you tenfold.
 

Offline Apollyon25_

  • Regular Contributor
  • *
  • Posts: 66
  • Country: nz
Re: What are the top "traps for young players" in basic PCB design?
« Reply #26 on: May 02, 2016, 08:45:11 pm »
On the topic of library parts, I'm not sure what capabilities other packages have, but Altium allows you to put the designator and comment (usually value/PN) as special strings in the component footprint, on whatever layer you like pre-arranged and pre-positioned.
This means for densely populated PCB's you simply can turn off the overlay layer (if you want) and have all the designator and values all set up on layers ready for printing/viewing. Saves you repositioning every piece of text on the board to be visible.
Print this layer really big, and with the BoM for qtys, hand placing is loads easier.

The other thing I do is create on a mech layer the physical body outline and a clearance area outline (IPC - N density typically), along with a centre of body crosshair and a pin one mark.
This lets me place components tightly together quickly, knowing I'm not going to have placement (machine) issues.
If I need to then nudge other components and test points closer I can see on the mech layer if there is any clearance issues from component bodies.
 

Offline basinstreetdesign

  • Frequent Contributor
  • **
  • Posts: 342
  • Country: ca
Re: What are the top "traps for young players" in basic PCB design?
« Reply #27 on: May 04, 2016, 01:58:25 am »
I must add one more bugaboo that seems to crop up any time I'm not watching and that is making sure that the footprint and pinout of three-terminal devices match between your schematic program and your PCB layout package.  This has happened I dont know how many times all during my career.   Take a 2n3904 transistor which has three leads and made by many manufacturers who do not agree how the pin numbers should be assigned.  If you use a 2n3904 from the schematic library and it gets linked to a TO-92 NPN transistor footprint from the layout library then those three leads have six different ways of being connected.  Chances are yours will be the wrong one.  If your design uses 24 of them and you are making 6 boards to start then you are in for a lot of re-work.

This kind of thing applies to diodes as well since the libraries may use pin numbers 1 and 2 or K and A.  As well the pin assignment for diodes can be screwed up by the same above issue.

Interestingly, as soon as the device in question gets four pins the problem seems to go away.

To guard against this kind of thing, make sure your PCB checklist (has anybody yet mentioned just how good having a checklist can be?) includes checking 2, 3 terminal devices for footprint against the datasheet by the actual manufacturer you will be buying your stuff from.
Tim
« Last Edit: May 04, 2016, 02:02:29 am by basinstreetdesign »
STAND BACK!  I'm going to try SCIENCE!
 
The following users thanked this post: alexanderbrevig, futurebird

Offline jolshefsky

  • Regular Contributor
  • *
  • Posts: 227
  • Country: us
    • Jason DoesItAll
Re: What are the top "traps for young players" in basic PCB design?
« Reply #28 on: May 05, 2016, 03:01:53 pm »
To guard against this kind of thing, make sure your PCB checklist (has anybody yet mentioned just how good having a checklist can be?) includes checking 2, 3 terminal devices for footprint against the datasheet by the actual manufacturer you will be buying your stuff from.

Good one. I should add that to my list.

My own libraries in KiCAD tend to lean on the "labeled" pins approach (e.g. BCE rather than 123). I think it's slightly more error resistant since if you take an NPN with pins named BCE and use a footprint with 123, none of the pins will be connected and it'll immediately be weird when doing layout. The trouble is the footprint count expands proportionally, what with the three order combinations and adding things like FETs and voltage regulators, all the sudden there's a lot of three-legged parts out there.

What would be needed, I think, is an intermediate step between schematic-part and layout-footprint where one maps the functional pins of a schematic to the functional pins in a specific device which THEN maps to the physical pins of a package. I should, then have just one TO-92 package in the library which could be related to any number of devices.

One thing I think was a win was to use C/NO/NC on all the switches in the libraries and footprints. So if I have a normally-open pushbutton in a schematic, it's got a common (C) and normally-open (NO) pin and I can use practically any switch as a footprint. Multiple poles get annotated starting at 1 (C1, NO1, C2, NO2, etc.)
May your deeds return to you tenfold.
 

Offline Cerebus

  • Super Contributor
  • ***
  • Posts: 4517
  • Country: gb
Re: What are the top "traps for young players" in basic PCB design?
« Reply #29 on: May 06, 2016, 01:32:14 am »
If you have enough layers, a ground plane will take away an enormous amount of pain in anything fast, sensitive or noisy. If you don't have enough layers use polygon pours for ground wherever you can.
Anybody got a syringe I can use to squeeze the magic smoke back into this?
 

Offline kendalll

  • Contributor
  • Posts: 21
  • Country: us
Re: What are the top "traps for young players" in basic PCB design?
« Reply #30 on: May 07, 2016, 09:32:08 pm »
Home etching a pcb seems like a waste of time and effort when there's options that are pretty affordable and reasonably good quality. https://oshpark.com/pricing

I mean unless the process of doing it at home is really fun for you...
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf