Industry Standard PCB Design Rules? - Page 1
Forum section: electronics / general

author: beaker353
author_rank: Unknown
timestamp: May 20, 2011, 02:13:28 am
content: I’m a hobbyist and EET student in the US that is trying to further my PCB design skills, amongst plenty of other design skills. I’ve used ExpressPCB in the past because of the good deal I can get, but I’m tired of their software restrictions and the inability to use the design files anywhere else. I now have the freeware version of Eagle that I’m slowly learning, and liking. I’m finding that the flexibility in regards to design rules within Eagle is both an asset and liability. For example, in ExpressPCB you were locked down to a set of pre-defined set of vias, plated through holes, and drill holes. This makes a lot of sense given that there are only so many drill sizes that can supported reasonably. In Eagle, I can choose just about any size, metric or imperial, in far many more increments than any manufacture would have. I imagine that if a fab house received a drill file with an odd size they would round it to the nearest drill and might charge an extra fee for use of drills outside a standard set.As I build my personal library of components, design methods, and such, I want to take the route that will make my boards both technically sound, inexpensive and practical to fabricate, and maximize the use of industry standards so near any fab house could produce one of my boards. Are there such a thing as industry accepted minimum design rules that everyone at least meets if not exceeds? It’s pretty easy to look at a handful of different board fabricators and get an idea, but I have a feeling that the collective brain of the forum might have something more concrete. Through hole sizes and simple drills are something I’m particular curious about as I have seen at least a couple of companies that clearly state they charge a per drill fee for each drill size they need to use that is not in their standard set. Not a huge deal if you are spitting out 1,000+ boards, but for one and two boards it can get stupid real quick. Best part is I can’t get them to tell me what their standard set of finished through holes and drills are. Grrr… I guess I’m magically supposed to know. Ideas anyone? Thanks!- EM

author: Mechatrommer
author_rank: Super Contributor
timestamp: May 20, 2011, 03:22:34 am
content: recently someone here suggested dipTrace. i downloaded and installed it, watch the online video guide, now i know diptrace alot more than eagle that has been idled for months in my pc. it also has 3d view (beta) which i'm yet to reach to that level. i'm looking forward for suggestion too.

author: beaker353
author_rank: Unknown
timestamp: May 20, 2011, 03:30:28 am
content: DipTrace looks interesting. I will definitely take a look. For right now though I’m going to probably stick with Eagle as it’s what my school uses exclusively. Regardless of what software package I’m using I believe that knowing the industry standards and keeping within them is important in the long run. Thanks Mechatrommer!- EM

author: RayJones
author_rank: Frequent Contributor
timestamp: May 20, 2011, 03:49:57 am
content: Generally drills are sized on 0.1mm increments, which roughly translates to 4 thou (thou = 1/1000th inch), or 4 mils as known in the PCB industry.It is generally not a good idea to expect an exact finished hole size, especially when plated through.With plated through, it is also a good idea to err on the bit larger size, nothing worse than header especially that won't fit in the holes, and drilling out is not really an option post event.Some design standards for through hole are:"12thou" = 62mil pads, 12mil track, 13mil clearance (typ 1 track between 0.1" spaced pads)"10thou" = 50mil pads, 10mil track, 10 mil clearance (typ 2 tracks between 0.1" spaced pads)

author: joelby
author_rank: Frequent Contributor
timestamp: May 20, 2011, 03:55:44 am
content: You can email PCB manufacturers and ask for a list of their standard drill sizes etc.Unfortunately their responses can be a bit cryptic sometimes - I tried asking about layer thicknesses once and didn't get an understandable response until I actually submitted a board and they queried my equally cryptic request for a particular stackup.

author: beaker353
author_rank: Unknown
timestamp: May 20, 2011, 09:27:57 pm
content: I emailed three fab houses about getting their specific drill and plated hole sizes two weeks ago. A week later I have an email from one saying "I'll get back to you", another with just "standard sizes", still waiting to hear back from the third. The idea though is I don't want to design to a particular fab house's specs. I've been caught more than one in a situation where I have designed something around a very manufacturer specific part that fits my requirements beautifully, but majorly screws me over when that company closes its doors and because it wasn’t an industry standard part, I have invest more R&D time. I would prefer to design to a standard that any house could fabricate to. That way I could choose which one meets other needs like time frame and cost.- EM

author: RayJones
author_rank: Frequent Contributor
timestamp: May 20, 2011, 10:28:06 pm
content: I've never had an issue sticking to drill sizes based upon the 0.1mm increment. Been doing PCB's for 20+ years with no reverse queries.0.8mm for most through hole components.0.9mm for headers1.0mm for power diodes (1N4001 style)A pair of calipers are your best friend to check lead sizes.How big a hole do you need? Some places will route larger holes and will usually specify the size at which this happens.Also there will be a minimum size as the drills are extremely fragile. Pushing below 0.4mm is pushing your luck.

author: johnmx
author_rank: Frequent Contributor
timestamp: May 20, 2011, 10:45:14 pm
content: This may help you: “Design Guidelines from Eurocircuits” (see pages 8 & 9):http://www.eurocircuits.com/images/stories/ec09/ec-design-guidelines-englsih-1-2010-v3.pdf

author: RayJones
author_rank: Frequent Contributor
timestamp: May 20, 2011, 10:56:43 pm
content: Quote from: johnmx on May 20, 2011, 10:45:14 pmLOL at bold text

author: Mechatrommer
author_rank: Super Contributor
timestamp: May 21, 2011, 01:30:13 am
content: Quote from: RayJones on May 20, 2011, 10:56:43 pmcambridge scramble style!

author: beaker353
author_rank: Unknown
timestamp: May 21, 2011, 02:29:30 am
content: So the consensus is there is no standards, great. Looks like I will need to find the secret password before I can get information from the fab houses. It's amazing how difficult it is to get basic specs from a company you want to give money to. It's not like it's some important trade secret which drills you use on your line.- EM

author: seattle
author_rank: Contributor
timestamp: May 21, 2011, 05:00:51 am
content: Design rules are a function of what you are willing to pay. If you use a PCBCart or SilverCircuits or just about any vendor that works on the web, they'll tell you the design rules right on their webpage. Use those rules, you get the quoted price. These can range from 7 to 4 mil trace, and 14 to 4 mil via. There's a huge range out there. And a large price delta. These guys are built for speed, so they will generally send you an email in a few hours if something in your board looks a bit too tight.I do cellphones for a living, and we do 10 layer boards with any layer laser via (ALIVH), 4 mil trace width. In these instances, we often start with a set of rules, but certain things might require some fudging of the rules. Because volumes are so high, the vendor will work to understand where the rules are being broken and they can sometimes slightly modify their rules. Sometimes, for example, when trying to route out of a 0.4mm pitch BGA, there might be places where the traces will thin to 3 mils. The vendor can accept this, they just need to know and understand.You note that you don't want to design to a particular fab house specs. If that is the case, then find 3 vendors you want to use, and use the loosest spec of all 3 and then you get a board that can run at all 3 no problems.I second the stuff others have written about diptrace. It's awesome. Eagle is like you are working on a 1988 DOS machine.

author: bartek
author_rank: Contributor
timestamp: May 21, 2011, 06:25:58 am
content: I just finished reading Dave's guide to PCB design and thought it was really good:http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

author: Bored@Work
author_rank: Super Contributor
timestamp: May 21, 2011, 06:50:11 am
content: Quote from: beaker353 on May 21, 2011, 02:29:30 amCompanies are not interested in the story of your life. The secret password is typically "I want to [buy|order] <huge quantity> of your <stuff>".

author: beaker353
author_rank: Unknown
timestamp: May 22, 2011, 01:26:14 am
content: Started playing with DipTrace last night after work. As I've been doing AutoCAD for many years the text based interface of Eagle didn't bother me in the least, but I have to admit that the logic in DipTrace feels better. A little more work up front, but better in the long run.I would say my three fab houses would be BatchPCB (looser tolerances, can do single boards), DorkbotPDX (tighter tolerances, but three boards required), and Advanced Circuits (for when I need a more than a handful). I'm doing small one-off projects with never more than a dozen boards or so, so I highly doubt that any fab house will see me as a big spender any time soon. My email to BatchPCB has gone completely ignored, the response from DorkbotPDX was "standard sizes" (again, secret handshake must be needed), and some sales rep from Advanced Circuits is supposed to get back to me, sometime.I just keep on going back to a project I did a few years back where I made some PCBs that fixed onto the backs of Socapex connectors (multi-pin connector used in theatrical lighting) to allow voltage measurements on these connectors in wall panels without interrupting the high current, high gauge wiring. There is no such thing as PCB mounts for these things so I designed some PCBs that fit around the base of the huge solder cups and then ran traces out to two Molex connectors. I used one house to fab the prototypes, then had a different house run the production due to budget restrictions (not my idea for the record). The first house fab'ed these huge though holes exactly as spec'ed, but the second house decided it was OK to drill down to the next standard size and completely hosed a $2,000 run. When I asked about this, they said their +/- .004 was to their standard drill sizes, not what I have spec'ed on the file. Had to personally eat a month's salary due to that error. Still a little bitter...- EM

author: Time
author_rank: Frequent Contributor
timestamp: May 22, 2011, 02:22:23 am
content: I usewww.freedfm.combefore I send off any board. Hobby or work

author: Mechatrommer
author_rank: Super Contributor
timestamp: May 22, 2011, 04:18:51 am
content: Quote from: beaker353 on May 22, 2011, 01:26:14 ami did with autocad too. but doing primitive stuff lines, circle to the exact coordinate accuracy is better and faster done in text based, even though there's toolbar for them, i still use text based. but for part replacement, track connection, pcb etc, thats different story.edit: drc is automatically check the error in pcb, never got into depth, but its there and in the video. will be usefull before sending to fabhouse.

author: Zero999
author_rank: Super Contributor
timestamp: May 27, 2011, 06:11:09 pm
content: Here's a few links:http://www.blackstick.co.uk/blog/?category_name=pcb-layout-tipshttp://www.ce-mag.com/ce-mag.com/archive/01/03/ProductSafety.htmlhttp://www.ce-mag.com/archive/01/Spring/Lamothe.htmlhttp://circuitcalculator.com/wordpress/2006/01/31/pcb-trace-width-calculator/