Different tolerances
Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=1618
Printed Date: 27 Jan 2025 at 5:20am
Topic: Different tolerances
Posted By: JJonas
Subject: Different tolerances
Date Posted: 24 Mar 2015 at 10:55am
In the picture below you can see two footprints that have the exact same name, but they look different.  |
Replies:
Posted By: Tom H
Date Posted: 24 Mar 2015 at 11:03am
|
You are absolutely correct. The IPC-7351 Land Pattern Naming Convention is starting to fall apart. We recommend a new naming convention - MfrName_MfrPartNumber This ties a component package directly to the Mfr. Part Number regardless of the component package tolerances. I meet with IPC at their headquarters the week of April 27th and this topic is on the agenda as we update the IPC-7351C Guideline. Yes, I said "Guideline". IPC-7351C will not be considered a "Standard" anymore. We voted unanimously on that at the IPC APEX meeting last month. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: JJonas
Date Posted: 26 Mar 2015 at 11:11am
|
Thank you for this insight. New naming convention will solve my reported issue, however, it will introduce two new inconveniences - duplication of footprints and inability to distinguish for which package a footprint is designed for. But I guess that is a trade-off. What about Step files, will IPC-7351C recommend using the same naming convention (MfrName_MfrPartNumber)? It looks like the old naming convention is still good, because tolerances have no importance (dimensions are nominal)? |
Posted By: Maarten Verhage
Date Posted: 26 Mar 2015 at 11:43am
|
Hello everybody, I do agree with fiaduu. Many many footprints are completely the same for different part numbers. I don't expect PCB designers like the approach of MfrName_MfrPartNumber. Having just a different speed grade for an FPGA requires to have a different footprint? I don't think many PCB designers will follow through. Maybe an addition can be made to the current IPC-7351 naming convention. Or maybe using an unique package description provided by a manufacturer. For example Lattice_PQFP208, if they can guarantee that once a 208 pins PQFP package is specified on their devices it is exactly that package. Otherwise THEY have to make a new unique name and STICK to that once and forever and tell the customers you promised to do that. That was my personal opinion. I hope PCB libraries allows discussions like this on this forum. Most of the times it is purely used for questions to PCB Libraries. Best regards, Maarten Verhage |
Posted By: Tom H
Date Posted: 26 Mar 2015 at 1:52pm
|
Let's put this in perspective. There are approximately 500,000 different component packages in the industry today and there will be more next year. When the IPC-7351 Naming Convention was created 12 years ago it was good for about 70% of all component packages. But as time goes by, component manufacturers continue to produce unique one-of-a-kind packages as to corner the market for their new IC that has multiple functions like Bluetooth, GPS, CPU processing, audio/video, etc. and you can remove 100 parts from your BOM and reduce the layer count by 4 - 6 layers if you single source this device. Are you going to do that? I think you might. So in 2015, the IPC-7351 Naming Convention is good for about 50% of all packages but quickly dropping. Most connectors are unique packages. Even the simplest USB connectors are produced with unique packages where the manufacturer is trying to corner the market with their connector. Connectors make up about 35 - 40% of all packages. And if most of them are unique, you can't use the IPC-7351 Naming Convention. Chip resistor packages by Panasonic might have a single package that maps to a couple thousand part numbers and this is good for the IPC-7351 Naming Convention. But what about multiple sourcing with AVX and Vishay? Do their 0603 package dimensions match Panasonic? Maybe, but it seems that the package Heights are all over the map. When 3D STEP modeling comes into play, having the perfect height becomes important if the PCB enclosure is tight. The new version of IPC-7351C has been downgraded from a "Standard" to a "Guideline". So there is no strict standard on footprint names. And we believe that 3D STEP model names, origins and rotations should match the footprint name. And, all the dimensions are nominal except for height. My vision of the future is that the IPC-7351 Naming Convention will eventually be phased out. Some of the names are already too long. A high pin count BGA could be as long as 40 characters. And the world standard for computer science names should not exceed 20 characters. This forum is open to discussions for anyone to openly discuss any topic. The standard needs to be challenged to insure that it's the best solution for the electronics industry. May the best ideas and concepts eventually win acceptance as the defacto standard. You can download the latest version of the Library Expert Naming Convention here. We tried to cover all the options. http://www.pcblibraries.com/products/fpx/userguide/default.asp?ch=5" rel="nofollow - http://www.pcblibraries.com/products/fpx/userguide/default.asp?ch=5 ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: JJonas
Date Posted: 27 Mar 2015 at 12:04pm
I think we need to separate unique and standard packages. For unique packages, I believe your suggested naming convention (MfrName_MfrPartNumber) is good. However, I still like the old naming convention for standard packages. I have just checked that there are ~1100 0603 resistors from Vishay on DigiKey and about the same number of 0603 resistors from Panasonic. MfrName_MfrPartNumber naming convention would not be very suitable for these parts because of extremely large number of duplicated footprints. One way of solving my reported issue with tolerances would be using maximum dimensions in footprint names, not nominal. This way we could continue using current naming convention for standard packages.
From my observations, most of the time no. And that is an issue - usually you need to create universal footprints for such simple components as resistors or capacitors. Personally, I would like to see a capability to combine several footprints into one universal within Library Expert. I have to do it manually now and it is a big time wasting activity.
I agree, but height is currently specified within Step file's name, for example CAPC2012X80. For this reason, I see no issues using current naming convention for Step files that do not involve unique packages.
Could you please provide a reference to this requirement?
Why don't you recommend adding Environment part to unique land patterns, i. e. MfrName_MfrPartNumber_Environment?
|
Tom H wrote:Posted By: Tom H
Date Posted: 27 Mar 2015 at 1:01pm
|
The character limitation was brought up in an IPC standards development meeting. I don't have the records of that meeting, but it was injected into the discussion by Dieter Bergman last year when we were reviewing an alternate Land Pattern Name solution. I'm not sure if he was referring to Cadence Allegro or some other CAD tool limits for both Land Pattern and Pad Stack names. When using the mfr. recommended pattern for unique packages, there is no guidance on a 3-Tier Density Level system. In this example of an International Rectifier footprint that is only 6 mm x 5 mm, see this datasheet pages 44 - 49 details on the pad, paste and solder mask sizes and locations. This FPX file for Library Expert took 4 hours to create and we sell it on http://www.pcblibraries.com/POD" rel="nofollow - www.pcblibraries.com/POD for a couple credits. http://www.irf.com/product-info/datasheets/data/ir3447m.pdf" rel="nofollow - http://www.irf.com/product-info/datasheets/data/ir3447m.pdf  ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Tom H
Date Posted: 30 Mar 2015 at 1:00pm
|
Update: I discussed the Land Pattern Naming Convention concerns in our weekly IPC-7351C development meeting today. Everyone on the executive committee agrees the short comings of the existing Naming Convention. One of the members from Germany recommended that we use an abbreviation of the Mfr. Name as a prefix followed by a hyphen. Example: TI-QFN50P350X350X100-19_15T205X205 This is the Texas Instruments QFN for the RHL case code. We have already collected every mfr. name and assigned an abbreviation and we'll be submitting it to the 1-13 Land Pattern subcommittee for review and comment. I'll let you know if this is accepted into the standard, but I personally approve it as it extends the life of the current naming convention. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Maarten Verhage
Date Posted: 30 Mar 2015 at 1:45pm
|
Hi Tom, Good to hear about that. I'm glad to see you seem to be willing to reconsider the initial idea of MfrName_MfrPartNumber. This discussion started with dealing with the different tolerances in the packages and the unique names for that. I think with the new idea it is important that the component manufacturers stick to their tolerances for the IPC-7351 Naming Convention names. I was wondering do you talk with component manufacturers about this? Would it be likely they are willing to commit to the new standard/guideline and promise not to mess with the tolerances or other dimensional data that might result in the same IPC-7351 footprint name but having different packages? About the IRF part you showed us. I would be trying to find another part that would give me this functionality rather than this overly complicated non-standard one. But it is great you also support packages like these in your software. Best regards, Maarten Verhage |
Posted By: Tom H
Date Posted: 30 Mar 2015 at 1:52pm
|
The new recommended IPC-7351C Land Pattern Naming Convention is only used for component families recognized in the IPC Standard and the Calculator. All unique packages and connectors created using FP Designer will use the MfrName_MfrPartNumber Naming Convention. And all complex one-of-a-kind packages will also use the MfrName_MfrPartNumber Naming Convention. Bottom Line is that regardless if the package is standard or unique, all Footprint Names will sort on the Mfr. Abbreviation and no longer sort by the component family abbreviation. Something that the IPC-7351C subcommittee must approve. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: jameshead
Date Posted: 07 Apr 2015 at 12:59am
For a standard naming land pattern having the manufacturer abbreviation as a suffix instead of a prefix would be better in my view, in sorting footprints in a library. When I'm looking for a standard footprint in a list I would prefer to see: SON80P400X400X80-9N-TI SON80P400X400X80-9N-AD So all the SON80Ps are grouped together. It kind of leads on better as the footprint name tells me from the beginning that it's a standard package, the size, then at the end that it's a Texas Instruments or Analog Devices variant. |
Posted By: Tom H
Date Posted: 07 Apr 2015 at 7:37am
|
We already thought of putting the manufacturer abbreviation as the Suffix, however, we're trying to have a universal naming convention that fits all parts created in FP Designer for Unique packages and connectors. Their naming convention is MfrNameAbvr_MfrPartNumber. We want ALL parts to sort by the component manufacturer abbreviation regardless if it is a Standard Part or a Non-standard Part or a Connector. Did you download the latest IPC-7351C Naming Convention Proposal - http://www.pcblibraries.com/forum/ipc7351-sm-footprint-naming-convention_topic479.html" rel="nofollow - http://www.pcblibraries.com/forum/ipc7351-sm-footprint-naming-convention_topic479.html You are suggesting that all "Standard" parts have the mfr. abbreviation as the land pattern name suffix and all "Non-standard" parts have the mfr. abbreviation as the land pattern name prefix. Or do you have a suggestion for the non-standard land pattern names? Or is this what you prefer? The 1-13 land pattern subcommittee will have to vote on this. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: jameshead
Date Posted: 07 Apr 2015 at 7:51am
|
Thanks Tom, I downloaded the latest copy from Dr Munie this morning. Last Friday and Monday were a bank holiday here in the UK. The Manufacturer_Manufacturer'sPartNumber naming is very sensible for non-standard parts and I can see the sense in extending it to standard footprints. I find it neater when viewing a list of land patterns in the CAD Tool's libraries to have ALL the same standard land patterns listed together though - and then easier to manipulate. In terms of looking at a standard land pattern name and "processing" the name in my head: I'm more interested in seeing if it's a standard land pattern, then what type it is, then what size it is, and to be honest I'm not bothered who the manufacturer is until the end. If that makes sense! I just wanted to add my tuppence halfpenny worth. If the agreement is to do it the other way around then that's what I'll do. |
Posted By: jameshead
Date Posted: 07 Apr 2015 at 8:06am
|
I just want to add something - when I'm outputting my centroid data for the assembler with the footprint name I am telling them importantly that it's a standard land pattern so they know the appropriate rotation (for us, Level A). For the assembler, they might only be interested in the SOIC127P600X...-3N bit and if it was at the front of the land pattern name it's easier for them to see. If they see something different at the front then it's a bit more of a red flag to say "hang on, this is a non-standard footprint - lets double check everything". Just a thought. It would be interesting to get some feedback from assemblers and auto-insertion programmers. |
Posted By: Tom H
Date Posted: 07 Apr 2015 at 8:16am
|
That's a good idea. All IPC Calculator parts have the mfr. abr. at the end of the land pattern name. All Unique parts that use the mfr. recommended pattern have the mfr. abr. at the beginning of the land pattern name. This way when you look at the land pattern name you know instantly if it's IPC-7351C calculation or mfr. recommended pattern. We're looking at adding common sense to the land pattern name. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |