| Author |
 Topic  |
|
KevL
United Kingdom
77 Posts |
 Posted - 05 Aug 2010 : 10:06:52
|
quote:
If issue 1 is resolved by combining the schematic/footprint/ component data into one component (the solution I am proposing) then issue 2 is solved .... thats my point.
I cant see that the above statement is true. Maybe I'm being dumb (quite possibly).
You have multiple components each with its own private copy of a say SOT-23 PCB footprint.
After Ive made (say) 98 components containing the SOT-23 footprint
I notice one of my SOT-23 pads needs to change size (say). How do I avoid having to open each component containing the SOT-23 footprint and editing it??
Kev
|
 |
|
|
Iain Wilkie
United Kingdom
459 Posts |
Posted - 05 Aug 2010 : 10:23:32
|
Why would you want to change the footprint pad size ?
If it needs to be altered for a particular design simply edit it in the design ... simple.
Iain
|
|
|
|
KevL
United Kingdom
77 Posts |
Posted - 05 Aug 2010 : 10:35:26
|
I wouldn't want to change the footprint at all but I might be forced to by having a change of PCB board assembly house. Their process might want different pad sizes.
Also it might not be pad sizes that need to change, Might be silk screen clearance from pads due to different design rules, requirment, soldering temperature profile. Any number of reasons that production engineers use to justify their salaries and cause electronic engineers to do the job twice.
Most assy houses say the the IPC footprints are a good place to start then hand you a list of the changes they cosniderer essential for high yield. Total pain in the bbackside but there you are. Maybe it is only high volume assy houses that are that choosey but there really are good reasons to have to change footprint after the event.
Changing footprints at PCB level is a horrible bodge. An uncontrollable mess.
If the footprint pads need changing they need to be changed in the libs so that next time a PCB is designed no one has to remeber to bodge the footprints after placement.
Kev
|
Edited by - KevL on 05 Aug 2010 10:35:44 |
|
|
|
Iain Wilkie
United Kingdom
459 Posts |
Posted - 05 Aug 2010 : 10:54:07
|
Kev,
In the 18 years I have done PCB layout for hundreds of customers with a dozen of different fab houses I have NEVER come across this.
Normally the Fab house will adjust the gerbers anyway to suit their process. If there is anything untoward in this , they contact and check.
Also if you DID change it all in the library, there is nothing to stop another manufacturer wanting it changed again etc etc,
Any changes for any particular design need to be local to that design.
Iain
|
Edited by - Iain Wilkie on 05 Aug 2010 11:11:32 |
|
|
|
KevL
United Kingdom
77 Posts |
Posted - 05 Aug 2010 : 11:09:50
|
Kev,
In the 18 years I have done PCB layout for hundreds of customers with a dozen of different fab houses I have NEVER come across this.
Then you have lived a charmed life and I am envious. I have worked for a number of companies where I used to dread the purchasing dept finding a new cheaper source of populated PCBs as it ALWAYS injvolved me or my guys having to dick around with data at the whim of some process engineer. Sometimes one had to wonder whether they had to change stuff just to prove they actually contributed to the job???
You might be insulated from it by your customer's production dept's or you have been dealing with smaller comanies with the "good" sense not to have to many QA guys etc.
Having fab houses mess with your gerbers is verboten by most companies with a quality system. They are making changes to co. data. The data has gone through design review process, version control, archiving. The output of some geezer with a scalpel may not have done. It is also recognised that if you have to post-process data to make it correct then you have to be really sure of the systems in place to ensure the post processing is always done. Will the guy who post processed last time remember to do it next time????
Quality systems .... dont you just love em.
Kev
|
Edited by - KevL on 05 Aug 2010 16:17:34 |
|
|
|
Iain Wilkie
United Kingdom
459 Posts |
Posted - 05 Aug 2010 : 17:59:41
|
Kev,
I wouldn't say it was a charmed life ... but it is a fact that this is not an issue I have come across to any extent.
Of cource there are always "tweeks" that need to be done after the first or even second spin but its never anything that causes a major headache.
Each Fab has its own set of design rules, and of course there are some generalities, but our designs tend to meet their criterion so there is never much of a problem.
I hear what you are saying about gerber adjustment ... and from the copper point of view there would always be a two way communication as there can be EMC and SI issues in that, but solder paste and resist apertures are sometimes brought into line with the particular processes.
Although a lot of the stuff I do is at the research and development level where quantities are not large .. I do have some major big players producing thousands of various layouts and really there is no problem along the lines you mention.
It could be that since your buyers are looking for cheaper supply, the lower cost board can suffer from a quality point of view and the the manufacturer needs to loosen tolerancies to reduce that cost and scrap to make it viable.
That did happen with one of our designs ... it was fine, changed manufacture to save money .... suddenly zero yeild, but rather than "edit" the tolerance errors out of the design, the client felt happier going back to the original supplier.
There is a lot of truth in you only get what you pay for !
Anyway I still think that one thing you do not want to be able to do is change a footprint globally in already designed components ....
Iain
|
|
|
|
KevL
United Kingdom
77 Posts |
Posted - 05 Aug 2010 : 20:03:21
|
Iain
Yes I agree with everything you have said re design rules being fab dependent etc, tweaks, needed resist appertures etc.
The other issue I come across a lot is that you actually need different footprints for some SM parts depending whether you are going to hand solder the first 10 prototypes and have production quantities machine assembled.
I've cocked that issue up more times than I'd like to admit. I open a datasheet, copy the footprint and think no more of it. Then when the boards come in my technicians bitch and moan that the footprints dont allow access to the pads by a soldering iron for hand assembly. i.e. pads are covered by part and are OK for paste and reflow but useless for hand assy. Out comes the solder paste , paintbrush and hot air blower - with attendent moaning from said technician.
Many SM inductors are like this - maybe because you do the layout job full time you dont make these daft sorts of errors.
Anyway we see the world differently re the below
quote:
Anyway I still think that one thing you do not want to be able to do is change a footprint globally in already designed components ....
I may be oversensitive on this issue but I have to say that I couldn't continue to use EZPC if I had to open a large number of components to modify what should be identical footprints. I would have to change PCB package.
I already have major issues with the difficulty in maintaining the libs. It might be the case that my company would be better off buying 4 seats of a considerably more expensive PCB package so that library maintainance would be faster - and hence more cost effective. Which is a pity because I really like the EZPC editor for drawing schematics and PCBs. It is fantastic value. Without disclosing proprietry info I'm sure you know what the charge out rate for design engineers in consultancy type companies is. £1000++ per day would not be far wide of the mark.
It simply isn't cost effective to have to spend vast ammounts of time hand editing components and having to do it in a number of components would only make this worse. As it is EZ PCB library primitives, styles, layers are very difficult to get working right - and almost impossible to get consistent - especially if, like us, you realise half way through using the libs that the way layers etc had been assigned was not working as well as it could. Our footprints have been designed to have silk screen outlines and also an accurate mechanical drawing layer so that we can export DXF and IDF data to solidworks. The way EZ PC is at the moment there is no alternative to opening up each component in a lib and editing say reference designator styles (the R and V symbols) there is no top level control. Now you might argue that maybe I should have worked out exactly what was needed before we got half way through drawing our libs - and you would be right - but we did try - just got it wrong.
In protel I can edit a footprint (say change line width of silk screen from 10mil to 8mil) and then apply that change to every part in the library - or all libraries i.e. it effectively does a search and replace of styles. In EZPC I have to open every part and do the job one at a time. This wastes hours.
This coupled with the need to hand edit component reference designators to ensure consistent contiguous numbering (to avoid phone calls asking why there is no R13 and R26 on the BOM - is this a mistake?) make some aspects of EZ PC very expensive to use.
Anyway I suspect we are not going to agree on this - though I'm certain that does not make either of us wrong. I hope you dont take my disagreement as a lack of respect - Just different ways of working and different needs etc.
Kev
|
Edited by - KevL on 05 Aug 2010 20:53:57 |
|
|
|
Iain Wilkie
United Kingdom
459 Posts |
Posted - 05 Aug 2010 : 20:56:03
|
Kev,
There is no dis-respect in anyway and none is taken ... more a lively debate that would be much easier done over an evening in the pub !. (and a lot more fun)
However two opposing views really due to two different working practices. This is were we need more users to join this debate to see which way it should be driven.
There are a few comments at the start of this thread, but latterly it seems to have been ourselves, which has perhaps been productive in airing two different opinions and kicking things off for a wider debate.
So lets hear from the rest of you guys, there are plenty of you out there. I think we agree the library structure has to change, but what does everyone else think...... ??
Iain
|
Edited by - Iain Wilkie on 12 Aug 2010 12:52:08 |
|
|
|
MikeMillen
United Kingdom
6 Posts |
Posted - 12 Aug 2010 : 09:15:54
|
I'd like to voice my support for Iain's proposal. It would represent a significant improvement to EPC, I believe.
A possible solution to Kev's objection would be if the Library Editor offered the option to globally find & change all instances of the changed symbol.
That way you can keep changes local or update the whole library.
|
|
|
|
neily
United Kingdom
3 Posts |
Posted - 12 Aug 2010 : 12:41:08
|
I too agree with Iain's proposed change to the libs and think that Mikes suggestion would be a good addition.
Has anyone from Number One commented on this yet?
|
|
|
|
jlawton
United Kingdom
35 Posts |
Posted - 17 Aug 2010 : 19:06:19
|
IMO the old system has become inadequate in the modern age with so many components available. I honestly don't see how it can be easily fixed as it stands.
I think that Pedro's proposal of a library system based on a database is the way to go. That way much more information can be related to each component, such as multiple vendor part numbers, and it could be searchable /sortable in different fields, etc. The relationship between schematic and layout parts would also be held in the database, and would be editable.
Look at Orcad Capture CIS as a way forward. http://www.ema-eda.com/resources/multimedia/RequestItem.aspx?itemID=193&campaignID=326 shows how the package has links to the component vendors.
See how new parts can be found then added to the local database: http://www.activeparts.com/walk-through.htm and http://www.activeparts.com/demo/activeparts.html
This looks like a better way forward from my point of view than vendor locked CAD packages like DesignSpark or the Advanced Circuits package.
Yes, I know EPC is a budget package!
BTW, why am I never offered an upgrade to the Pulsonix system, I think the sales side is missing a trick here :)
John |
|
|
|
KevL
United Kingdom
77 Posts |
Posted - 19 Aug 2010 : 11:00:38
|
Not really disagreeing with the above but maybe a few thoughts to stir into the equation re component libs and databases.
A populated PCB is usually a subassembly to a larger system. As such a BOM from a PCB will typically become part of a larger BOM which is typically managed by an MRP system. The rest of the BOM might come from multiple sources (e.g 3D CAD etc) Even if you sell populated PCBs there will be items in the product not fitted to the PCB (e.g. poly bag, manual, leads, labels etc). So unless you make schematics containing symbols for labels etc then EPC wont ever make a complete BOM.
The MRP system will usually contain purchasing info, description, supplier info cost etc etc.
There is NEVER a requirement for duplication of said info. If "SAME" info is in two places then it will be wrong in one of them because it will be impossible to keep the info the same.
So is an information rich database system nailed onto a PCB package really the way to go? Is the PCB package really the going to replace an MRP system???
I get the impression that many competitive products add lots of facilities to their packages because they have run out of ways to allow tracks to be joined to pads (E.g Protel). So you get bolt on poor mans MRP systems etc, 3d board viewers which guess what the parts nmight looklike, really poor mans 3d CAD etc. etc.
I would think the info in the libs should be the minimum to unambiguously identify a part in a schematic (for design and design review) and then in a BOM for export to MRP. I.e. keep EPC databse simple with low info content .... but the parts should reference external data and EPC should be capable of BOM output in a format that external MRP systems can deal with (CSV).
I think one of the main problems with the curent lib system is tht EPC designed a completely flexible system then failed to advise a preferred way to configure and use it. Hence many of the lib problems. |
Edited by - KevL on 19 Aug 2010 11:18:00 |
|
|
|
TheBFG
United Kingdom
61 Posts |
Posted - 20 Aug 2010 : 08:20:24
|
I don't think copying PCB footprint data into a component is a good idea. I don't think data duplication is ever a good idea and I guess thats why databases use more than one table!
The problem I have with the libraries is simply that there is more than one, and therefore names become non unique and it is possible to pull an incorrect (but identically named) PCB footprint from the wrong library.
I think one library, with partitions perhaps, and good import / export / update facilities is the way to go.
As for exporting and sharing components then I think yes all info should go in one file, but when it is imported some checking would need to be done to make sure the footprint and symbol names did not already exist in the target library. |
|
|
|
Iain Wilkie
United Kingdom
459 Posts |
Posted - 20 Aug 2010 : 09:27:10
|
In other words we would still have the same problem ... if there is duplicate information which is correct ?.
Having all the info within the component gets round this. Please note that you could (if you wish) edit/add to the footprint info within a component, but that would be under your control. Th problem arises at the moment when the component "looks" for its footprint in the libraries by name only and can (and has done in the past) applyed the wrong pinning !.
iain
|
|
|
|
TheBFG
United Kingdom
61 Posts |
Posted - 20 Aug 2010 : 10:43:48
|
I really don't think the solution is to duplicate footprint data in the component. This is generally considered bad practice, hence my comment on database design, and this is really a problem of database design.
Like you say the problem occurs because the SW looks for the footprint by name only, and there may be another footprint in a different library with the same name. There is not enough information (other than search order) to pick the correct footprint.
Possible solutions are
1. Use just one library - as long PCB footprint name is unique (i.e. primary key), no problem occurs.
2. If using multiple libraries, each footprint name in each library must be unique, and each library must have a unique identifer or name. The component then references both the PCB footprint name and the library name it came from. |
|
|
|
Topic |
|
Library Structure Suggestion
