Re: [PEDA] SMT resistor array footprints and usage?
As everybody else has indicated, you are best to create your own. I'll assume you are getting your parts (or at least have seen the parts) in a Digikey catalog. I've used the footprints for the Panasonic EXB-A and EXB-V8V footprints as they are called out in the catalog and they worked fine. As somebody else suggested, unless you are doing reflow soldering you may have some continuity problems with the cupped leads these packages offer. Great for reflow, bad for inspection or hand soldering. Bryn Matt Polak wrote: Hey all, Rather dumb question here, but I'm stumped. Can someone enlighten me as to where the footprints for surface-mount chip resistor arrays are, and how I would set them up against my schematic? I want to use something like an EZA or EXB series resistor array to help cut down on component count/size in a rather demanding layout, but I can't seem to find anything other than the standard discreet SMT footprints (1206, 0805, etc) that I've been using thus far. Any help would be greatly appreciated. I assume that I must be missing something stupid. -- Matt -- Name : Bryn Wolfe Title : Robotics Engineer Dept : Texas Robotics Automation Center (TRACLabs) Company: Metrica, Inc Addr : 1012 Hercules Drive Houston, TX 77058-2722 Voice : 281-461-7886 NASA : n/a FAX: 281-461-9550 Web: http://www.traclabs.com Email : mailto:[EMAIL PROTECTED] or mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SMT resistor array footprints and usage?
Hey, you guys rock! : Thanks so much to all of you for the helpful feedback concerning the resistor question I posted the other evening. Doing a handful of designs layouts in Protel thus far has been a big learning experience, I can defiantly say I agree with creating the custom footprints/landpatterns that multiple folks mentioned. After getting a DB25 connector footprint back on a prototype featuring 30 mil holes for the mechanical locking clips (ouch!) rather than something more like 90's, I have been extremely careful with double-checking all footprints I lay down. It's good to know that most folks simply prefer to create most footprints from scratch rather than hunting them down. Glad to also hear that I wasn't just missing something or doing something wrong - you usually tend to assume it's a problem with the user when commercial software doesn't act as it's supposed/intended to. : Also, thanks for all of the varied responses, suggestions, and comments concerning the resistor arrays, suggestions for footprint layout, laser-printer 1:1 prints for double-checking, manufacturing suggestions, and all of the other amazingly helpful material. I really wish I'd found this list sooner! Very best regards, -- Matt * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SMT resistor array footprints and usage?
At 04:00 PM 14/01/02 -0500, you wrote: Hey all, Rather dumb question here, but I'm stumped. Can someone enlighten me as to where the footprints for surface-mount chip resistor arrays are, and how I would set them up against my schematic? I want to use something like an EZA or EXB series resistor array to help cut down on component count/size in a rather demanding layout, but I can't seem to find anything other than the standard discreet SMT footprints (1206, 0805, etc) that I've been using thus far. Any help would be greatly appreciated. I assume that I must be missing something stupid. -- Matt It really is very little problem to make your own footprints, once you take the time to learn how (and there is help in the manuals). What is harder is having the experience to sort of judge what will work when you have no guidelines. If you can find a manufacturers recommended layout then you can easily transfer this into a Protel library. I suggest you create new Sch and PCB library documents and look about for suitable footprint data from a couple of manufacturers and then take the time to learn how to create both Sch symbols and PCB footprints. Then you can look at existing Sch and PCB libraries for ideas/suggestions on how footprints are created. For PCB footprints you probably only need to add a number of top layer surface pads (that is hole size of zero) and some tracks on the top overlay to give the bounding rectangle. The size and position of the pads comes from the manufacturers data - usually it is not given in the centre-to-centre format that you will need for Protel and so some subtractions and additions may be required. As far as the overlay goes, creating the bounding rectangle is often where I am most fussy as big outlines are really clumsy but if they are too small then they do not show (adequately) the required manufacturing clearances and/or you risk overlay drifting onto the pads when there is manufacturing mis-registration. I usually keep overly about 8 mils wide and at least 10 mils from pads - sometimes further depending on what mood I am in. I am fairly sure I created the 1206 quad-Res footprint we use from manufacturers suggested layout so such info must be around. Doing a 1:1 laser plot, centred on the page, can be a useful check if you are nervous. As for Sch symbols - these are also easy enough to create but there is more info that can be entered into the library. I strongly suggest that you take the time to understand the different pin types and be religious about assigning the correct pin type to each pin. This will make ERC reliable. Also, entering in details such as the default designator etc will also speed your later work. Make sure you choose a naming scheme that is unlikely to conflict with existing components as this can cause problems - less so than in the past though since the component cache matching has been tightened up. With a resistor array you have the choice of making a multi-part component or putting all the array elements together. This choice depends largely on your Sch style and preference. There is also help in the manuals on creating Sch symbols. Once you have created the library parts do not forget to add them to the library list of the Sch and PCB documents you are editing. Remember a library document that is open for editing is not necessarily available in the library list for other documents. Sorry is the above is old hat and you already new all of it. But the faster that Protel users realize that they are not constrained by the existence of components that happen to be in the Protel supplied libraries the better. (Many people swear off any packaged libraries, preferring to at least carefully check pre-prepared symbols and footprints very carefully before use and then extracting/modifying into their own validated library system.) Bye for now, Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SMT resistor array footprints and usage?
I'm afraid you'll probably have to make the footprints. As I'm sure I won't be the last to tell you: it's dicing with death (of the project) to use Protel supplied footprints. There are a large number of footprints in error to a greater or lesser degree. Every single footprint used should be carefully checked against the manufacturer's published component mechanical specification (there's also a wide variance in manufacturer to manufacturer dimensions for the same nominal package). If ever I'm tempted to use a pre-existing Protel footprint I get up, go have a drink and remember what happened the last time I did so :-( , then go back to my desk and do the job properly (i.e. build a new footprint from scratch or by modifying one of my own previous creations. Cheers, John Haddy -Original Message- From: Matt Polak [mailto:[EMAIL PROTECTED]] Sent: Tuesday, 15 January 2002 8:00 AM To: Protel EDA Forum Subject: [PEDA] SMT resistor array footprints and usage? Hey all, Rather dumb question here, but I'm stumped. Can someone enlighten me as to where the footprints for surface-mount chip resistor arrays are, and how I would set them up against my schematic? I want to use something like an EZA or EXB series resistor array to help cut down on component count/size in a rather demanding layout, but I can't seem to find anything other than the standard discreet SMT footprints (1206, 0805, etc) that I've been using thus far. Any help would be greatly appreciated. I assume that I must be missing something stupid. -- Matt * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SMT resistor array footprints and usage?
i agree with John's view here the supplied footprints are not all bad or entirely worthless but given that you should check all footprints and put them in a verified_footprints lib, the amount of work to make one is similar to the amount of work to thoroughly check one also there are widely varying standards and practices regarding hole size and other issues smd res paks come in a lot of sizes and shapes, the paste dots can be very small, so the footprint design should be verified with your assembler i've had a bit of trouble with those being soldered properly, esp the kind with the little cups at the edges, they are also hard to visually inspect between those issues single sourcing issues and routing issues i am starting to shy away from them altogether after being a long time advocate of the component count reduction they offer Dennis Saputelli John Haddy wrote: I'm afraid you'll probably have to make the footprints. As I'm sure I won't be the last to tell you: it's dicing with death (of the project) to use Protel supplied footprints. There are a large number of footprints in error to a greater or lesser degree. Every single footprint used should be carefully checked against the manufacturer's published component mechanical specification (there's also a wide variance in manufacturer to manufacturer dimensions for the same nominal package). If ever I'm tempted to use a pre-existing Protel footprint I get up, go have a drink and remember what happened the last time I did so :-( , then go back to my desk and do the job properly (i.e. build a new footprint from scratch or by modifying one of my own previous creations. Cheers, John Haddy -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
