Are certain "IPC compliant" nom. footprints with oversized pads really worth it? - Page 1
Forum section: electronics / projects

author: incf
author_rank: Frequent Contributor
timestamp: May 28, 2025, 11:25:46 am
content: QuoteQuoteSee imageoriginal question (which has been clarified above):Are "IPC" compliant footprints with huge pads really worth it? It can make it hard to fit traces and vias between the rows of pins.At first glance I feel that the manufacturer's footprint ("MFG") is more 'correct' than the IPC one. I feel like they might be assuming larger tolerances than actually are common.addendum, an example of some wild pad geometries:

author: tszaboo
author_rank: Super Contributor
timestamp: May 28, 2025, 11:36:04 am
content: SOT-25 is not the same as SOT23-5. Pitch is different. So use the correct footprint.Otherwise, there are 3 levels of IPC pads in Altium. L, M, N, with difference in pad sizes. Use the one most appropriate for your design.

author: incf
author_rank: Frequent Contributor
timestamp: May 28, 2025, 12:19:44 pm
content: Quote from: tszaboo on May 28, 2025, 11:36:04 am(honest question) How different are they?For some reason I seem to have convinced myself that they might have the same pitch and row center-line spacing. Even after going back and checking I'm still a bit unsure about differences between SOT-25 and SOT23-5 - except for maybe tolerances. But I could be misreading the drawings (or even looking at the wrong ones).

author: wraper
author_rank: Unknown
timestamp: May 28, 2025, 12:30:30 pm
content: Quote from: tszaboo on May 28, 2025, 11:36:04 amThey have exactly the same dimensions.

author: tszaboo
author_rank: Super Contributor
timestamp: May 28, 2025, 02:04:24 pm
content: Quote from: incf on May 28, 2025, 12:19:44 pmActually, SOT25 seems to be a Diodes specific naming of SOT23-5.I think I confused it with SOT523.

author: incf
author_rank: Frequent Contributor
timestamp: May 28, 2025, 02:56:16 pm
content: Is there any real benefit to the huge pads the "IPC" footprint? They seem too big to me. Far outside of the tolerances I'd expect.Why does the manufacturer's footprint use such small pads?

author: UnijunctionTransistor
author_rank: Frequent Contributor
timestamp: May 28, 2025, 03:44:10 pm
content: From google;IPC standards areindustry-recognized guidelinesdeveloped to ensureconsistency and qualityin electronics manufacturing.Bolding mine. But these are the key words. Very important key words.I see these standards as an industry wide know-how. They are not mandatory requirements, but only suggestions acquired through collective blood, sweat and tears. As such they are very conservative, and you can ignore them and your products may still be fully functional and compliant.But my 45+ years in actual electronics manufacturing, tells me that whenever these guidelines are followed, significant pain and suffering is avoided in the future.Not only that, but if you plan to assemble these boards thru a contractor, and you start having repetitive problems, the contractor very likely will play the your-board-not-meeting-IPC card and refuse responsibility.And I know that I will get replies here along the lines of “I have never followed IPC and never had an issue”. To which I reply, You are one lucky guy. You must be the same person who purchased a Ford vehicle with the original three-cylinder Ecoboost engine and driven it for 200,000 miles without problems.

author: incf
author_rank: Frequent Contributor
timestamp: May 28, 2025, 03:53:05 pm
content: The question is not really about "should I use IPC"It's about justifying variation between difference sources of footprints.I can find you a dozen different "IPC" footprints for the same parts. Some nominal IPC footprints have pads that are way too big. Some nominal IPC footprints appear to have normal pads.It seems to me that the parameters used to autogenerate some of these footprints are not realistic.I'm am hoping to identify if there are any valid use-cases for what appear to be 'obviously incorrectly generated' nominal IPC footprints. Do any parts exist that actually claim large enough tolerances to justify such oversized pads?As far as I can tell, in my designs, I should be deleting my nominal IPC footprints that contain oversized pads, and replacing them with correctly generated nominal IPC footprints.

author: UnijunctionTransistor
author_rank: Frequent Contributor
timestamp: May 28, 2025, 04:07:01 pm
content: Again, IPC guidelines are only MANUFACTURING suggestions.And these suggestions will depend whether your circuit is consumer grade, industrial grade, medical grade or aerospace grade.There can’t be a single one-size-fits-all criteria.Dumb example: there were millions and millions of VCRs manufactured with paper-phenolic boards. But would you use them for a jet-engine fuel computer?

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 28, 2025, 04:56:59 pm
content: When I search for SOT25 I get a very old fashioned THT transistor package.If you want to compare sizes, just put them next to each other on the PCB. For posting a screenshot, add a ruler for scale.Rounded corners in pads have a clear advantage. They reduce the amount of solder paste that can get stuck in the corners of the stencil, and therefore the amount of paste deposited on the pads is more consistent. Bigger pads allow for easier rework, while smaller pads enable higher density and therefore smaller PCB's.

author: ajb
author_rank: Super Contributor
timestamp: May 28, 2025, 07:54:30 pm
content: Quote from: UnijunctionTransistor on May 28, 2025, 03:44:10 pmThe standards aren't just conservative, it looks like they're pretty old -- IPC-7351B was released in 2010. Electronics have changed a lot in the last 15 years, and so has assembly equipment to keep up with the kinds of boards that are being made nowadays. The accuracy of component placement and consistency of solder paste application (including in very small amounts) have to be much better for modern high-density designs and smaller packages, and that will trickle down to more pedestrian SOT and SOIC parts as well.Is there a more up-to-date standard? I wouldn't be surprised if there isn't just be cause the pace of change over the last decade has been too rapid for a proper standards-making process to keep up with.Quote from: UnijunctionTransistor on May 28, 2025, 03:44:10 pmMaybe I've been lucky, but the CMs I've worked with have all been very good about pointing out potential issues before manufacturing, and I would certainly expect them to work with me to solve a recurring assembly problem. Even if it does boil down to my footprints being wrong, I wouldn't want to keep working with a CM who can't point that out and tell me what the actual issue is so I can fix it -- they're supposed to be the assembly experts after all! And FWIW, I've had CMs point out that a footprint doesn't match the component manufacturer's recommendation, but in the last 10 years I've never had one point out that it doesn't match IPC recommendations. YMMV of course.

author: IconicPCB
author_rank: Super Contributor
timestamp: May 29, 2025, 06:35:38 am
content: Horses for courses... what soldering process do you use, air convection... wave soldering.. vapor phase reflow.. robotic with soldering iron, with laser, hot bar soldering etc etc etc...

author: hfleming
author_rank: Regular Contributor
timestamp: May 29, 2025, 02:26:43 pm
content: Around 20 years ago, IPC footprints were mandatory for the avionics designs I worked on. We also redesigned a very complicated product that was not IPC-compliant, that had a 90% reject rate after PCB-assembly. Just by redesigning the PCB’s to adhere to IPC-standards, we had less than a 5% reject rate.

author: incf
author_rank: Frequent Contributor
timestamp: May 29, 2025, 02:32:06 pm
content: Quote from: hfleming on May 29, 2025, 02:26:43 pmThe question is not really about IPC, but rather how certain "IPC compliant" (it quotation marks) footprints are generated. "What assumptions are baked into what appear to be wildly oversized versions of nominal IPC footprints? Is there any justification for them, or was it simply that no care went into generating them?"

author: Siwastaja
author_rank: Super Contributor
timestamp: May 29, 2025, 03:41:09 pm
content: Quote from: incf on May 29, 2025, 02:32:06 pmYou are getting specific enough with your questions so that you should just read the standard.

author: tooki
author_rank: Super Contributor
timestamp: May 29, 2025, 03:59:40 pm
content: Quote from: tszaboo on May 28, 2025, 02:04:24 pmNo, definitely not specific to Diodes, Inc. I found examples from Diodes, Microchip, Torex, Rohm, Toshiba, and some Chinese vendors. Appears to be equivalent to SC-74A and SC-95, which have different thicknesses, and SOT753.See also:https://www.rohm.com/package-page?searchkeyword=sot-25(What a mess…)

author: ejeffrey
author_rank: Super Contributor
timestamp: May 29, 2025, 04:37:39 pm
content: Quote from: incf on May 29, 2025, 02:32:06 pmAs explained, IPC-7351 provides multiple different options for sizing based on density requirements. The appropriate choice depends on your manufacturing needs and your board density.The only information you have shown is two footprint images that are obviously scaled differently, contain no dimensions, and don't reference the part or manufacturer recommendation that your are considering. You have also not said which options you selected when generating the IPC footprint. So basically nobody can say anything useful about it.I haven't found the IPC-7351 "nominal" footprints to be excessively large. They are reliable for reflow assembly, provide good fillets for strength and to avoid stress concentration, and are relatively easy to rework. You can absolutely use tighter footprints, at some cost.I generally don't like to use manfuacturer footprints simply because different manufacturers will often recommend different footprints for the same package with no apparent reason. I would rather not have multiple different SOT23-5 footprints depending on whether I am using a TI part or an analog devices part. Consistent footprint sizing helps manufacturing as it's easier to tune your paste application and reflow profiles if everything uses similar fillets.

author: incf
author_rank: Frequent Contributor
timestamp: May 29, 2025, 04:46:19 pm
content: Quote from: ejeffrey on May 29, 2025, 04:37:39 pmThese "nominal" IPC footprints are provided by the manufacturers. (ie. of the three options: least, nominal, maximum - they allegedly use 'nominal' IPC settings)

author: ejeffrey
author_rank: Super Contributor
timestamp: May 29, 2025, 04:51:20 pm
content: Can you post the *(&$# data sheet you are looking at and the dimensions, otherwise this is just a waste of everyone's time.Are you saying the manufacturer provided two footprint options and you like one better than the other? If they provided two options you will need to ask them why. Or is the footprint you called the "manufacturers footprint" not actually provided by the manufacturer and you just invented it?

author: Siwastaja
author_rank: Super Contributor
timestamp: May 29, 2025, 06:30:16 pm
content: Quote from: tooki on May 29, 2025, 03:59:40 pmFootprint naming is a lost cause. Luckily, they are often unnecessary: during design, find suitable parts, see drawings if it fits, draw footprints and 3D models according to the drawings, use existing footprints only after manually checking for equality, or not at all. In a workflow like this, the name of footprint is irrelevant.But one thing where you can't avoid them is when finding compatible alternatives. Then you need to know all >10 aliases to find as many suitable parts as possible from parametric searches, and still miss some.

author: incf
author_rank: Frequent Contributor
timestamp: May 29, 2025, 06:39:56 pm
content: Probably 20% of the footprints in Altium's manufacturer part search are a bit wonky.The most recent example of this is the following:The 2N7002W-7-F from Diode's Inc.When I look at the manufacturer's provided footprint lineup I think "something is not quite right" - the pads are almost touching, and go too far under the body.I speculate if these were generated by hand with an IPC wizard that the dimensions of the pads would differ significantly.That begs the question: "is there really value in these massively oversized pads when compared to more typical pad sizes?"It has nothing to do with "IPC" and everything to do with assumptions about manufacturing tolerances that seem to go far beyond the dimensional tolerances of the component in question. I get the "larger pads are easier to rework" argument. But is there really any value in the pads going so far under the body of the part?I always use the "nominal IPC" footprints recommended by the manufacturers, but in some cases they are just too "absurdly oversized" to be able to route traces between the pads.

author: harerod
author_rank: Frequent Contributor
timestamp: May 29, 2025, 07:47:51 pm
content: Quote from: incf on May 29, 2025, 06:39:56 pmhttps://www.diodes.com/part/view/2N7002W/#Are you complaining about some obscure Altium library or the datasheet?

author: ejeffrey
author_rank: Super Contributor
timestamp: May 29, 2025, 07:54:19 pm
content: Quote from: incf on May 29, 2025, 06:39:56 pmI don't know how those get there and I don't generally use that. For standard SMT packages I use the IPC footprint wizard in Altium and enter the physical lead dimensions from the data sheet. For non-standard parts like connectors I either use the manufacturers footprint generator tool or draw it by hand.There is only one footprint in the data sheet for that part:https://www.diodes.com/assets/Datasheets/2N7002W.pdfand it exactly matches the manufacturers separate "package information" document:https://www.diodes.com/assets/Package-Files/SOT323-Standard.pdfSo your "IPC" footprints are not "manufacturers recommended IPC footprints" they are "footprints you downloaded from an online database alleging to be generated by the IPC rules"QuoteI strongly recommend you do that. That's the only thing worth talking about.QuoteI don't know how far it should go. That's definitely something to watch for on narrow components where two rows of leads are close to each other. You still want a fillet there, but it's certainly possible that it's more than you need. On the other hand, I doubt it would actually cause a problem. My preference would be to stick with the IPC-7351 recommendations, generating the footprint myself unless I had a reason other than "I don't like that"

author: tooki
author_rank: Super Contributor
timestamp: May 29, 2025, 08:09:35 pm
content: Quote from: incf on May 29, 2025, 02:32:06 pmThey aren’t just “assumptions”, never mind “no care”, IPC footprints use mathematical formulas to determine the footprint geometry. So typically, one enters the key dimensions of the package into a piece of software, which then generates the IPC compliant footprints according to those dimensions and the formulas.https://resources.altium.com/p/pcb-land-pattern-design-ipc-7351-standard(summary)https://www.ipc.org/system/files/technical_resource/E31%26S01-3_Dieter.pdf(more detail)Quote from: incf on May 29, 2025, 06:39:56 pmLarger pads give more leeway for misalignment during component placement, meaning you can use a faster, older, or otherwise less precise PNP machine. Larger pads also have more area to bond with the board, potentially improving reliability in some situations. (And yes, improving ease of hand-soldering, too.)Quote from: incf on May 29, 2025, 06:39:56 pmWhy not try it out and find out? It’d be interesting to see if Altium’s IPC generator produces similar or differing output from what’s in the Altium Vault.(Also, let me express a gentle reminder that just because the reason for something isn’t evident or knownto youdoesn’t mean that a sound reason doesn’t exist.)

author: UnijunctionTransistor
author_rank: Frequent Contributor
timestamp: May 29, 2025, 08:20:57 pm
content: Quote from: tooki on May 29, 2025, 03:59:40 pmThat was the understatement of the week.

author: Siwastaja
author_rank: Super Contributor
timestamp: May 30, 2025, 02:19:31 pm
content: Quote from: tooki on May 29, 2025, 08:09:35 pmExactly! Simply, don't trust libraries, don't download footprints - generate them yourself with e.g. Altium's IPC-compliant footprint generator. It still is garbage in garbage out, but at least the "in" part is the manufacturer's mechanical drawing of thepart itself- which is way more reliable than the recommended footprint drawing!Basically the only thing I have watched out for are parts with excessive mechanical tolerances. Like, manufacturer wants for liability reasons specify that their body width may vary between 3mm and 5mm, but it really isn't going to vary that much. Excess tolerances lead to excessively large pads that go long under the package. So when I see ridiculous tolerance values, I take a brief look at competitor's part in the "same" package to get an idea what isactuallytypical, and reduce the given tolerance a bit.One thing I learned within recent component crises which come and go is to look for second-sourceability during initial design, not as afterthought. When you do this, you also will have several datasheets open already, so good opportunity to compare dimensions, tolerances and footprint suggestions.You learn bit by bit what is important. But IPC-compliant (least if you are space-constrained) from original manufacturer drawings is the safest initial bet. There is a reason why pads need to go longer "below" the package; if you remove too much material there, self-alignment during reflow suffers and you can end up with tomb-stoning. You CM will then curse as they have to manually fix 5 boards out of 100.