Author Topic: IPC footprint naming correct?  (Read 1676 times)

0 Members and 1 Guest are viewing this topic.

Offline PJ Bain

  • Contributor
  • Posts: 15
  • Country: au
IPC footprint naming correct?
« on: August 06, 2020, 11:25:48 pm »
I have been tasked with auditing our verified libraries, and have noticed a discrepancy with the way the Altium IPC Footprint wizard names components.

For example... according to IPC 7351B (which Altium apparently follows) an 0402 0.56mm high chip capacitor medium density would be named CAPC1005X56N. Altium names it CAPC1005X06N.

Is there some rational behind this or have I misunderstood the standard? Otherwise we are going to have to rename all Altium generated footprints to correctly reflect the IPC standard. Which I think we'll end up doing anyway as it is more accurate.

Cheers
Pete
 

Offline envisionelec

  • Frequent Contributor
  • **
  • Posts: 271
  • Country: us
Re: IPC footprint naming correct?
« Reply #1 on: August 07, 2020, 01:38:24 pm »
I have been tasked with auditing our verified libraries, and have noticed a discrepancy with the way the Altium IPC Footprint wizard names components.

For example... according to IPC 7351B (which Altium apparently follows) an 0402 0.56mm high chip capacitor medium density would be named CAPC1005X56N. Altium names it CAPC1005X06N.

Is there some rational behind this or have I misunderstood the standard? Otherwise we are going to have to rename all Altium generated footprints to correctly reflect the IPC standard. Which I think we'll end up doing anyway as it is more accurate.

Cheers
Pete

I think the general consensus is that Altium IPC generates IPC Compliant footprints, but the naming is generated according to their own algorithm. I see you also posted to Altium Support Forums, so I did a search there and found addditional commentary on this topic including a link to a guide that is quite thorough and might be helpful to understand what Altium is doing.

https://confluence.desy.de/display/ALTIUM/Footprint+naming+convention
 

Offline PJ Bain

  • Contributor
  • Posts: 15
  • Country: au
Re: IPC footprint naming correct?
« Reply #2 on: August 10, 2020, 01:27:27 am »
Thanks for the reply and link. Very useful to know.

Yeah I haven't had any issues with their footprints, and I like the fact their 3D body generator is to max dimensions all round (and quite nice looking components), but the naming does seem a little hit and miss.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7653
  • Country: us
    • SiliconValleyGarage
Re: IPC footprint naming correct?
« Reply #3 on: August 10, 2020, 03:07:43 am »
depends on the number of digits

technically it should be CAPC1005X056N. Altium rounds so it becomes CAPC1005X06N

CAPC 1.0mm 0.5mm X 0.6mm thick

but then again. IPC is no longer a standard. only a guideline .... the C version took so long to make it is already obsolete. Many in the industry are abandoning IPC as they lag behind terribly on the technology curve.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Online dunkemhigh

  • Super Contributor
  • ***
  • Posts: 2875
Re: IPC footprint naming correct?
« Reply #4 on: August 10, 2020, 01:31:47 pm »
Quote
Many in the industry are abandoning IPC

What's the preferred replacement?
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7653
  • Country: us
    • SiliconValleyGarage
Re: IPC footprint naming correct?
« Reply #5 on: August 10, 2020, 04:56:07 pm »
Quote
Many in the industry are abandoning IPC

What's the preferred replacement?

manufacturer , manufacturer part number.

There are simply too many new footprints for which IPC has no naming convention.
Same thing for packages with thermal pads. They have no defined nomenclature.

I have 6 package names

dual row :

SO : small outline
SOT : small outline transistor
SON : small outline no pins

quad :

QFN : quad flat no pins
QFP : Quad flat pins
PLCC : you know.

syntax : <type> pitch <p> length <x> width <N> pincount [<TH> length x width ]   ' squre bracket is optional. if there is a thermal pad : give its dimensions.

Anything that can not be encoded  like the above ( dual thermal pads , double rings , whatever ) becomes manufacturer-manufacturer partnumber-manufacturer package name.

TI-TUSB3310-DRG0008

Done. IPC can sod off. There have been hefty discussions about this on multiple forums. One of the IPC council directors even admitted : just use manu/manu part. disk space is cheap and it solves many problems.
There are too many permutations. SOT23 .. you need at least 8 or 9 to accomodate the differences. Do you really want such a library ? it is going to be hell when you start working with alternates.
Technically there is only one SOT23. problem is it costs money to license that design. So everybody mickey-mouses it... on very dense designs it is an issue.
I spent years mucking it out. i now have 1 SOT23. 1 SOT24 one SOT25 one SOT26

Even the manufacturers fuck it up royally. Here is a DFN14. That is impossible. DFN : Diode Flat NO lead. DFN is the no leads variant of a SOD or SOT . 2 or 3 pins max !

i have two buckets : pins and no pins.
and each has dual and quad configs.

done. it makes my searching for a fooprint very easy

Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: zeke, Alex Eisenhut

Online dunkemhigh

  • Super Contributor
  • ***
  • Posts: 2875
Re: IPC footprint naming correct?
« Reply #6 on: August 10, 2020, 06:10:53 pm »
Thanks :)
 

Offline chris_leyson

  • Super Contributor
  • ***
  • Posts: 1513
  • Country: wales
Re: IPC footprint naming correct?
« Reply #7 on: August 10, 2020, 07:56:00 pm »
Thanks free_electron. IPC naming is OK for a lot of generic parts SO, SOT, SON etc. but I like the Manufacturer = Part = Manufacturer Package Name convention, it makes a lot more sense. Thermal pads really screw up IPC naming conventions. Package size is another issue to watch out for, I've seen a few designs where some opto-couplers would barely fit on the PCB because of their wider package and someone had used a generic footprint, would have been safer to use the manfacturers part number. Also seen production PCBs fail where someone had used the smallest SOT-23 footprint I've ever seen, if you placed the part spot on centre you could maybe get a heal fillet under each leg but a lot of time the middle leg wasn't even touching the pad.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7653
  • Country: us
    • SiliconValleyGarage
Re: IPC footprint naming correct?
« Reply #8 on: August 11, 2020, 02:56:53 pm »
exactly. Things are too different.
- use manufacturer suggested footprint
- encode always the toe-to-toe space an thermal pad size

- Do NOT trust names such as MSOP VSOP TSSOP. TI is a total fuck up. they have a package handbook that call out VSOP is down to 0.65mm pitch . MSOP is 0.5mm and then they release parts with VSOp with .. 0.5mm pitch ... so they violate their own package handbook.
- ALWAYS look at the measurements and work from there.
- Beware of Toshiba . they have non standard body widths and lengths. TI also has a few non-standard body widths.
- anything coming from DIODES needs to be studied very critically. Diodes is the BORG of the semiconductor world. They have absorbed so many companies that they have incompatible packages in their line-up . they are cleaning it up now which leads to another problem : as they are unifying the packages all of a sudden there are issues with parts that were fine in the last 10 years. they still have 5 different SOT23 's ... SOT23 is a JEDEC standard. THERE IS ONLY ONE ! if it deviates it is not a SOT23 ! Pay the goddamn royalties on the package and move on. All this SuperSot, Tsot ,SOTplus is all garbage invented to circumvent the copyrights.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: zeke

Offline Feynman

  • Regular Contributor
  • *
  • Posts: 112
  • Country: ch
Re: IPC footprint naming correct?
« Reply #9 on: September 13, 2020, 08:07:27 am »
IPC is no longer a standard. only a guideline .... the C version took so long to make it is already obsolete.
As far as I know it has not even been published yet. And probably never will be due to fluctuation in the working group's personnel.

My suggestion would be to follow the naming convention of Tom Hausherr's library tool ("Library Expert"):
- <Mfg>_<Mfg Partname> (e.g. for connectors) or
- <Mfg>_<Mfg Case Code> (for special packages) or
- Library Expert's naming convention for generic footprints, which are an improvement to the IPC naming convention.

The Library Expert Naming convention even has a long list of manufacturer name abbreviations to be used in footprint names ("ONSEMI" for On Semiconductor, "TI" for Texas Instruments, "ANALOG" for Analog Devices, ...).

Example for a generic footprint: "RESC320X160X140L50N" for a 3,2mm (nom. length) x 1,6mm (nom. width)  x 1,4mm (max. height) 0,5mm nom. lead length medium density chip resistor.

I don't think it is convenient to name ALL footprints after Mfg+Partname/Package. Just think of the slightly different sizes of chip resistors: A Yageo 0603 might have slightly different dimensions than a Panasonic 0603. Chances are you prefer one single footprint that is a compromise to fit all 0603 resistors.

I don't know if I'm allowed to publish the Library Expert naming convention here, but you can download it from www.pcblibraries.com. Or just use Library Expert to generate footprints and import them in your CAD tool.
« Last Edit: September 13, 2020, 12:19:49 pm by Feynman »
 

Offline exmadscientist

  • Regular Contributor
  • *
  • Posts: 234
  • Country: us
Re: IPC footprint naming correct?
« Reply #10 on: September 13, 2020, 09:02:06 pm »
My suggestion would be to follow the naming convention of Tom Hausherr's library tool ("Library Expert"):

Please don't use this incomprehensibly verbose convention. Library Expert is fantastic and gets so many things right, but this isn't one of them. It solves the easy problems for you, and makes the harder part of the problem worse, keeping you reliant on Library Expert for help.

When you're assigning footprints to components, there are two things to check:
  • Have I selected the right footprint for this component?
  • Is that footprint drawn correctly?

So for your 0603 resistor, problem 1 is making sure that you pick an 0603 footprint instead of 0402 or 0306 or 0805 or whatever. Then problem 2 is making sure your 0603 footprint in your library is good for actually soldering an 0603-sized part to. #2 is more difficult: drawing good footprints can sometimes take a while. And they must be maintained, for example when library standards change. In contrast, #1 is really easy: just read the datasheet and pick out the correct footprint from your library. The rub is that you must do operation #2 once per footprint you draw; you probably have dozens to hundreds of footprints. But #1 applies per component, and you have thousands to tens of thousands of those!

Library expert makes #2 super easy: it draws perfect footprints perfectly well. It makes #1 very difficult, because it assigns stupid names that cannot be quickly audited. If you are using a SOT23-5 op-amp from TI, with TI package code DBV, and I see that the assigned footprint is "JEDEC MO-178 AA (SOT23-5)", I'm happy! If I see "TI DBV-5", I'm also happy! If I see that footprint "SOT23-5P95_280X145L45X40" has been assigned, I... have no idea if that's right. I mean, sure, it looks approximately correct, but those are the worst to audit... is 280 correct? 145? I don't know. Time to spend some quality time with TI's drawing, I guess :( .

So it's relatively easy to check that footprints named this way are drawn according to their names. It's quite difficult to check that they are assigned properly to parts, and because that is the more common task, I strongly dislike this approach to library organization. Instead I prefer:
  • Draw as many footprints as possible to standards (JEDEC, JEITA, EIA, ... ). Qualify manufacturer packages as equivalent to these standards, which is usually quick and easy (and we have a database that saves the association), and then you can use one standard footprint to replace a dozen or more manufacturer footprints. Name them as suggested above: by the standard and by the common name: "JEDEC MO-178 AA (SOT23-5)".
  • When official standards do not exist (or are practically unobtainable, like EIA passive sizes) and defacto standards exist, take a few minutes to define a GENERIC footprint that covers 95+% of the market and use as above. Example naming: "GENERIC SOT-89" or "CHIP RES EIA 0603/1608M".
  • Nonstandard or oddball parts are, if reused at all, usually only reused within one manufacturer. So draw them up as manufacturer-specific, and index them by manufacturer: "TI DBV0005A" so the next time you're stuck using a DBV0005A from TI you know you've already got it covered. This also works fine if you don't recognize something as standard... it's just a footprint tailored to one vendor. Nothing wrong with that.

The actual drawing of the parts can be handled by Library Expert... I just never use its names, because I cannot audit them as being correct to apply to parts. My goal is to draw as few footprints as possible, of as high a quality as possible, and use them as often as I can. This way, if you change op-amp vendors but keep the same part, you won't be stuck with a silly tool telling you the footprint ought to change by a few microns!
 
The following users thanked this post: dunkemhigh

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7653
  • Country: us
    • SiliconValleyGarage
Re: IPC footprint naming correct?
« Reply #11 on: September 17, 2020, 06:14:31 pm »
The problem with libraryexpert is that it generates footprints without regard for, or understanding of, your manufacturers capabilities. Courtyards is one issue. How close can you place parts for your manufacturing process ? your courtyards are important for that.
Thermal relief structures ? windowpane soldermask ? lattice paste mask ? unheard of.

I stopped using it 5 years ago for many reasons. Use the suggested landpatterns from the datasheets. and create a uniform pattern for the commodity stuff. like SOT23. Oh, and NEVER EVER trust the names manufacturers assign to their footprints.
Here is a VSSOP10 ... with 0.5mm pitch ... nope. xSSOP is 0.65. MSOP is 0.5 .... or a DFN10 . there is no such thing as a DFN10. A DFN package has 2 or 3 pins. Not more. Those packages are called SON.

As for naming IC packages <type><pitch><toe-to-toe>-<pincount>-[thermal pad size]

SOP50P490-10-TH120x140   : so package 0.5mm pitch , 4.9mm toe to toe , 10 pins with a thermal pad of 1.2 by 1.4 mm
QFN40p900x900-76-th340x340  : QFN 0.4mm pitch , 9 by 9 mm , 76 pins , 3.4 by 3.4 mm thermal pad

and so on

i also have SOT23 SOT24 SOT25 in the library. in the descriptor field i add the alternate names such as SOT23-3 SOT23-4 SOT23-5 SC74 and manufacturer specific names if i know them. Next time i need a footprint : simply search for *whatever and it will pop up if you have it.

Works like a champ. 1
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: zeke


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf