Standardized footprint references

Thank you for your suggestion and taking the time to reply :)

Ivan

Brad,

Thank you for taking the time to present such a detailed and informative reply. I greatly appreciate your effort and advice.

Ivan

I have seen pad dimensions in various PCB CAD programs for a number of SMT parts, and the dimensions were said to come from some standard (which i will not mention). I have even seen some nicely done drawings used to justify some of the dimensions of those pads. Suffice to say, that pad dimensions go all over the map, from being smaller (one or both dimensions), thru exactly the size, to excessively larger than the part lead that would be soldered onto that pad - especially when one looks at different parts that have the same exact lead size. So, as far as i am concerned, the "standard" is not too useful or functional. In short, make the lead pads any size you want.

If it were me, i would make *recommendations* and/or *guidelines*, since nobody seems to give a damn as to what the term "standard" is supposed to mean. Start with the pad exactly the size of the lead that would go onto it. Optionally, add to those X and Y dimensions, any or all of the following:

1) Add a mil or two for positioning errors. 2) On the edge where a lead bends down toward the solder pad, add one to three mils for solder meniscus. 3) Add one half of a mil, to one mil for solder meniscus from a given lead edge to solder pad. The above three recommendations or guidelines then would give a minimal pad size that would be workable in almost any shop.

Leon

--
Leon Heller, G1HSM
http://www.geocities.com/leon_heller

Ivan, Take a lot of the information you gain here with a grain of salt. I don't know where Robert gained his experience but by his comment on allowing for meniscus he must have been dealing with

3-6mil high parts/leads. 1 - 3 mils heel length is totally inadequate for a normal real world part. He was kinda right about the IPC land pattern standard, one cannot design land patterns allowing for the wide variation of manufacturers dimensional allowances as IPC suggests (i.e. an SOIC lead foot length of 14mil - 50mil, use 32mil as the real length +/- 18mil but forget the tolerance when designing the land pattern. Do you ever see a SOIC foot vary by more than 3 times the minimum length in the real world?). Their system does work pretty good if you design for the median part dimensions and drop the min and max cases. SMT Plus' system says the same thing, forget designing for the max and mins.

I have to think that Robert was talking about a SOIC type lead but he doesn't state so. Besides SOIC leads there are a large and varied number of pad requirements for various devices. Some of those requirements are for soldering, some are for test and some are for reworkability, good pad designs are a blending of all three. By the way, for a standard common SOIC lead I would use 20mils on the toe and heel of the lead, the heal for solder joint strength (meniscus) and the toe for somewhere to get your heat into the pad for rework (also works well for a test probe point). (i.e. a 12mil wide SOIC lead with 22mils of foot, a pad

14 - 16mils wide and 62 mils in length, centered on the centerpoint of the lead's foot. On small pitch SO devices (also QFPs, LCCs, TSSOPs and all other small pitch devices) the pad width will approach the same width as the lead, i.e. 8mil lead width, pad - 8-9mil width. Sometimes the gap between pads can take priority over the pad width and drive the pad width right down to matching the lead width.)

There are too many issues to discuss in this forum but I would suggest that you look at SMT Plus' literature. I know that he had two books that he used to sell that discuss land patterns for SMT devices and runs through a lot of the rules to designing good SMT land patterns. I have used SMT Plus' system for about 12 years now, it has never let me down through many companies and across numerous assembly shops.

As for your question about Protel patterns and where to find them, I don't know because I never use canned libraries. On that note be warned that Protel libraries do have errors in them. Some errors are significant, not just borderline issues. Protel does have some sort of a library listing on their website if I remember correctly and it is still there. It might be an interactive utility or spreadsheet.

--
Sincerely,
Brad Velander

"Ivan"  wrote in message
news:t10e11h4n0e4e0m0bup0226qvouqjuegpq@4ax.com...
> Thank you for your suggestion and taking the time to reply :)
>
> Ivan
>

IPC-SM-782 is a good starting point. They have an on-line calculator which is unpleasant to use.

Check manufacturers data sheets and application notes.

AVX has done extensive research on chip capacitors and land patterns. Look for their "Surface Mounting Guide" for MLC chip capacitors. I like using their reflow dimensions.

PCB Standards has a landpattern calculator. It designs to IPC-782 standards. Check out pcbstandards forums > PCBstandards > Free Resources > Library Part Documentation for some good info.

Mark

Mark-

Thank you! The urls that you provided answered many questions, including those for reflow and wave soldering specs.

I appreciate your attention and help.

Thank you once again,

Ivan