Author Topic: Good(?) PCB and SMD footprint design guidelines  (Read 11765 times)

0 Members and 1 Guest are viewing this topic.

Offline Zom-BTopic starter

  • Regular Contributor
  • *
  • Posts: 55
  • Country: nl
Good(?) PCB and SMD footprint design guidelines
« on: February 22, 2017, 11:16:19 am »
By accident I stumbled on this page with PCB design guidelines for manufacturabiility: http://www.altronmfg.com/pcb-design-for-manufacturability/

It mainly focuses on SMD pad design, which is exactly what I needed because all the other guidelines I've ever seen (before and after I found this) only focus on the PCB, assuming footprints are already made.

Now I have to wonder (since I only have one reference so far), what do other people think of these guidelines? Good, bad, biased, domain-specific? Is there a better (non-book) source for similar information?
 

Offline DavidMenting

  • Contributor
  • Posts: 45
  • Country: nl
    • Nut & Bolt interaction design
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #1 on: February 22, 2017, 09:00:45 pm »
Tom Hausherr's blog might give you more than you asked for: https://blogs.mentor.com/tom-hausherr/

He goes into detail on pretty much all aspects of SMD footprints.
 
The following users thanked this post: ar__systems

Offline ar__systems

  • Frequent Contributor
  • **
  • Posts: 516
  • Country: ca
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #2 on: February 23, 2017, 12:08:31 am »
that's a really good document
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 22397
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #3 on: February 23, 2017, 02:13:33 pm »
Also, IPC-7351 is freely available.  It documents standard package and footprint types, how they are dimensioned and toleranced, and recommendations on how to dimension the footprints.

Meanwhile, do read up on mechanical drafting terms and methods; modern datum + variance methods look cryptic, but are quite concise and powerful, once you know what they mean.

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline Mattylad

  • Regular Contributor
  • *
  • Posts: 143
  • Country: gb
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #4 on: February 28, 2017, 07:33:16 pm »
Er, no it is not. (not legally).
IPC-7351 costs wollah (money) and the only freely available copies are not actually very helpful in making your footprints.

Better to get the Library Expert (the Lite version is freely available) from pcblibraries.com which will make your footprints for you, based on the dimensions you enter from the datasheet and spit the output to almost any PCB package, no need to read a boring standard, let the tool calculate all the solder joints for you.

Also, IPC-7351 is freely available.  It documents standard package and footprint types, how they are dimensioned and toleranced, and recommendations on how to dimension the footprints.

Meanwhile, do read up on mechanical drafting terms and methods; modern datum + variance methods look cryptic, but are quite concise and powerful, once you know what they mean.

Tim
Matty
CID+
 
The following users thanked this post: montemcguire

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 22397
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #5 on: February 28, 2017, 09:41:35 pm »
Er, no it is not. (not legally).
IPC-7351 costs wollah (money) and the only freely available copies are not actually very helpful in making your footprints.

Please at least try...
e.g.
http://pcbget.ru/Files/Standarts/IPC_7351.pdf

(Whether that source is legal or not, is up to IPC, I guess.  And whatever laws "pcbget.ru" happens to be under, which, well...)

Section 3 fully specifies how to calculate footprints from part dimensions.  I don't know how to get any more helpful than "fully specified". :)

Quote
Better to get the Library Expert (the Lite version is freely available) from pcblibraries.com which will make your footprints for you, based on the dimensions you enter from the datasheet and spit the output to almost any PCB package, no need to read a boring standard, let the tool calculate all the solder joints for you.

Also a fine method, though, using any tool blind leads to the same result: GIGO.  One must always think about the values they are entering, and for what purpose they serve.  To that end, the discussion by IPC provides this illumination, for those willing to see it. ;)

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline Mattylad

  • Regular Contributor
  • *
  • Posts: 143
  • Country: gb
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #6 on: March 01, 2017, 01:51:48 pm »
That's an older version, (also an illegal\copyright infringement)  the current one is B - about to be replaced by C.

Most engineers I know of prefer to save time when creating footprints, use the free tool that is to the IPC spec and makes them for them, quickly and with far less chance or errors than someone doing it
BY all means obtain the standard, but I'd use the tool myself - just like I use a tool to layout a PCB and screw wires into a terminal block.
It is also recommended by the IPC themselves.

However, if doing it the hard way is what floats your boat - go for it.
Matty
CID+
 

Offline tszaboo

  • Super Contributor
  • ***
  • Posts: 7910
  • Country: nl
  • Current job: ATEX product design
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #7 on: March 01, 2017, 02:48:06 pm »
That's an older version, (also an illegal\copyright infringement)  the current one is B - about to be replaced by C.

Most engineers I know of prefer to save time when creating footprints, use the free tool that is to the IPC spec and makes them for them, quickly and with far less chance or errors than someone doing it
BY all means obtain the standard, but I'd use the tool myself - just like I use a tool to layout a PCB and screw wires into a terminal block.
It is also recommended by the IPC themselves.

However, if doing it the hard way is what floats your boat - go for it.
Most engineers I know just use the Altium built in IPC compliant footprint wizzard...

(Whether that source is legal or not, is up to IPC, I guess.  And whatever laws "pcbget.ru" happens to be under, which, well...)
No it is not legal. Russians have no concept of what the word "legal" means.
 

Offline montemcguire

  • Regular Contributor
  • *
  • Posts: 88
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #8 on: March 25, 2017, 01:59:03 am »
I'll second the recommendation for PCB Library Expert software. While it's not perfect, it can make some extremely high quality footprints. It's not terribly difficult to use, assuming you can get proper dimensions for your components. For some poorly defined parts, I've used a USB microscope to measure actual parts, and also to verify dimensions that seem a little odd.

The basic idea is that each part will have its own footprint, based on the dimensions and tolerances that are unique to that vendor's part. This means that there is no such thing as a generic SO8 or a 2012 chip. So, you need to create specific footprints from the dimensions of each part. But, if you do this, the footprints very closely fit the specific part, making assembly extremely reliable.

Because each part needs its own footprint, it can take some time to get a complete library. But, that seems to be par for the course with PCB CAD anyway - I no longer trust any footprint unless I create it myself. The process is finite too, so it can just take some time but the results will be excellent.

One good point is that many IC vendors have a range of packages that get reused among some set of devices, so there really isn't one footprint per device, but instead, one footprint per vendor package. Once you get a footprint for the likely packages you'll use from a vendor, you can make any of their parts from these footprints easily.

Bottom terminated components are the most troublesome these days, especially those with irregularly shaped die attach pads, but the nice version of PCBLE includes a Footprint Designer which allows you to do pretty much anything you want. Plus, a part can be started using the standard calculator and then altered, possibly to add an unusual DAP, or to provide some odd pin numbering scheme.

Again, PCBLE is highly recommended over studying the IPC documents.  http://www.pcblibraries.com/LibraryExpert/
 

Offline westfw

  • Super Contributor
  • ***
  • Posts: 4306
  • Country: us
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #9 on: March 28, 2017, 06:20:10 am »
So since the topic has come up...
In several common EAGLE libraries, the SMT packages for a resistor, capacitor, and LED, all in (say) a 0805 SMT package, are slightly to significantly different.  In some cases, it looks like there were two footprints for a resistor (one for wave soldering, one for reflow?), and only one of them was copied to the (ie) LED library, but in other cases, there are stranger differences...

Is this expected?
 

Offline bitwelder

  • Frequent Contributor
  • **
  • Posts: 972
  • Country: fi
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #10 on: March 28, 2017, 12:21:33 pm »
So since the topic has come up...
In several common EAGLE libraries, the SMT packages for a resistor, capacitor, and LED, all in (say) a 0805 SMT package, are slightly to significantly different.  In some cases, it looks like there were two footprints for a resistor (one for wave soldering, one for reflow?), and only one of them was copied to the (ie) LED library, but in other cases, there are stranger differences...

Is this expected?
Is it because it's following this guideline? 
Robert Feranec: "TIP #055: Use different footprint for resistors and capacitors, even they are same size (e.g. 0805)"
 

Offline timb

  • Super Contributor
  • ***
  • Posts: 2536
  • Country: us
  • Pretentiously Posting Polysyllabic Prose
    • timb.us
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #11 on: March 28, 2017, 12:34:36 pm »
One good point is that many IC vendors have a range of packages that get reused among some set of devices, so there really isn't one footprint per device, but instead, one footprint per vendor package. Once you get a footprint for the likely packages you'll use from a vendor, you can make any of their parts from these footprints easily.

Yeah,  this is good advice. A lot of IC manufacturers (TI, Linear, Analog, etc.) will have specific, non-standard codes for their packages, so that's how I label them in my library.
Any sufficiently advanced technology is indistinguishable from magic; e.g., Cheez Whiz, Hot Dogs and RF.
 
The following users thanked this post: montemcguire

Offline timb

  • Super Contributor
  • ***
  • Posts: 2536
  • Country: us
  • Pretentiously Posting Polysyllabic Prose
    • timb.us
Good(?) PCB and SMD footprint design guidelines
« Reply #12 on: March 28, 2017, 11:17:43 pm »
Yes, that is the best way.
I find that it is risky to just create something like "SOT23-3" without great care and assume it will work for any manufacturer's implementation of it. 

In particular I've seen cases where the toe / heel / side spacings that were somehow created (not by me) to accommodate one manufacturer's package GDT was not at all right for another manufacturer's package of the "same type".

I imagine that mechanical compatibility as it relates to the footprint could/should be better if they're all tied to some set of JEDEC package type parameters if those give the true GDT for the entire range of compatible packages and are the basis of your footprint design, but if you just create one based on vendor A's GDT, don't expect it'll generate a good IPC footprint for vendor B or vendor C's packages.

And by the time you consider things like package height or 3D model you're really on thin ice trying to make a generic one size fits all footprint.  Whereas a vendor specific one will / should work for everything from that vendor in that package code.

Of course it seems like some vendors have multiple different package codes / drawings for the same basic package, I assume some of that may be due to things like changing lead frame tools / suppliers or handling ceramic vs. plastic or lead free vs not or something but it doesn't do the CAD librarian any favors in trying to create a comprehensive library and then trying to figure out if the flavors of packages even from a single vendor and package type are really footprint compatible.

There have been (somewhat standard) cross tool standards for representing SPICE models, S-parameters, IBIS data for a long time.  One would think that there long ago should have been a standard mark up language for IC package GDT data and particularly recommended footprints so one can just paste a little file snippet into one's CAD tool and get the MCAD aspects of a footprint defined along with an example footprint.  Same with pin naming and pin numbering for that matter.
One could say that STEP or IGES are "standard formats" though it seems like even among MCAD tools they're horror stories of "incompatibility" so it seems like something that's a well defined subset or something ad-hoc would be better.

At any rate it is bloody ridiculous that it is 2017 and we're manually typing in (not even copy & paste!) dimensions from some shoddy PDF's MCAD sketch at the bottom of a data sheet to make footprints and manually typing in pinout table data from badly formated tables elsewhere in the PDF to get the schematic symbol defined.  Literally ANYTHING would be better.

It is a rarity (maybe 15%?) that you even get IBIS / STEP files or ASCII .TXT / EXCEL pinout files from IC vendors.  You'd think that they never actually 'feel the pain' of using their OWN tools / documents to use their own parts.  If you're lucky and you have a matching CAD system you'll get Allegro / Altium / Eagle or whatever CAD libraries from the IC vendor though even there you still end up with some questions of style compatibility and concens about correctness.  It would be nice if there was something that actually represented "the specification" for the part's MCAD / ECAD in a portable manner so that it could be cross checked against CAD library implementations as well as used to guide wizard derived implementations.

IC vendors are still living in the 1980s.  They've got oh so "pretty" "flashy" web sites downgraded annually, but by and large they do not a single thing to actually make using their parts with CAE/CAD tools by standard or at least facile mechanisms meaningfully easier.

Yeah,  this is good advice. A lot of IC manufacturers (TI, Linear, Analog, etc.) will have specific, non-standard codes for their packages, so that's how I label them in my library.

Exactly. It's mind boggling there's no standard to define footprints. There needs to be one standard, plaintext file that includes: Footprint information, pin names and 3D data (STEP could be used here, as it's already plaintext, IIRC). You download the single file and import it into your ECAD software's library. The STEP file could be automatically (and easily from a code point of view) split out of the single file and saved to wherever you keep your 3D models.

By the way, to clarify, I think that for a hobbyist who is just hand soldering SMD parts to small boards, the default footprints in most affordable ECAD software (Diptrace, Eagle, CircuitMaker, Etc.) is alright to use, as those packages generally have oversized pads to aid in hand soldering. For example, the standard DipTrace patterns (SOT-23, SOIC, TSSOP, SMD caps and resistors, etc.) work just fine for pretty much any package from any vendor if you're using a soldering iron or hot air gun.

Where you need to worry about custom footprints for each specific package is when you're going to be manufacturing the boards in quantity.

I bring that up only because I don't want someone working on their first board to come across this thread and think it applies to them.
« Last Edit: March 31, 2017, 01:48:19 am by timb »
Any sufficiently advanced technology is indistinguishable from magic; e.g., Cheez Whiz, Hot Dogs and RF.
 

Offline senso

  • Frequent Contributor
  • **
  • Posts: 951
  • Country: pt
    • My AVR tutorials
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #13 on: March 31, 2017, 12:41:56 am »
Just yesterday I made the footprint for a small push-button 4 direction "joystick" from ALPS, the dimensions are in a little corner of a PDF and are some crappy jpg image that will get blurry AF if I try to zoom in, reading some numbers is almost impossible.

And I also do a new footprint for each variation of SOT-xxx and assign it to its respective component, there are always variations of 0.x mm in pad sizes, I thought I was kinda stupid to do it and that there should be some standard/universal size, guess I'm not that dumb  :-+
 

Offline exmadscientist

  • Frequent Contributor
  • **
  • Posts: 404
  • Country: us
  • Technically A Professional
Re: Good(?) PCB and SMD footprint design guidelines
« Reply #14 on: April 01, 2017, 07:01:41 am »
If you're drawing your footprints for the common packages to a manufacturer's drawings, you're wasting your time. (Unless you're in high-volume manufacturing.) You should be using the JEDEC package reference documents, which most manufacturers are compliant with. (But not all! Never blindly trust without verification.) As an example, you could copy the manufacturer's recommendations (or use IPC/PCB Library Expert when land patterns are not provided) to draw up the following "SO-8" packages:
  • TI D (R-PDSO-G8)
  • NXP SOT96-1
  • ADI R-8
  • LTC S8
  • Intersil M8.15
  • Fairchild M08A
  • Maxim S8-fifteendifferentmoreorlessidenticalsuffixes (have I mentioned lately that I hate Maxim?)
However, all of the above explicitly state compliance with JEDEC standard MS-012-AA (except LTC, who are compliant if you check the drawings yourself). So you could instead draw one MS-012-AA SO-8 footprint, take the time to verify it thoroughly, and be done. Which do you think has a greater chance of happening: you making half a dozen almost-identical footprints flawlessly, or a major manufacturer delivering parts so far out of spec that they won't solder to a standard footprint?

And, honestly, if your process is so sensitive that the differences between the manufacturers' different footprints is making a noticeable difference in your yield, you probably have something wrong anyway. Most of those drawings above have identical basic dimensions and vary only in their tolerancing -- not to mention that there's a decent chance the parts are all coming off the same packaging subcontractor's production line -- so if you can actually tell the difference, you really should figure out what's happening and fix it.

(This cost-benefit analysis does, of course, break down for very high-volume manufacturing. But if you're doing that, you should have the resources to test everything and be discussing things in detail with your assembly people.)

Once you've settled on a single standardized footprint, you still have to deal with making sure it gets correctly assigned to the right parts. I use Altium database libraries, and found that I could set up the database to do most of the work for me. I set up a single packages table with manufacturer package code as a primary key, and fill in all relevant package-specific information in that table. That includes the manufacturer name, common name, dimensions, applicable JEDEC standard, and the reference to the footprint location in my PCB libraries. I then reference this table by a foreign key in the actual parts tables, so all I have to do is fill in the manufacturer code there and, once I've got that package code entered correctly once, the database automatically returns the package information with the part data when Altium queries the database. The information is stored in only one place, making it easy to get right and easy to update later if it's not (or no longer) right. This system took a while to set up but it's invaluable when dealing with things like the thicket of single-gate logic packages.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf