How should several toleranced dimensions be added together to make a footprint? - Page 1
Forum section: electronics / general

author: montemcguire
author_rank: Regular Contributor
timestamp: August 11, 2021, 11:29:49 pm
content: I've been happily using PCB Library Expert to generate footprints for components, and I have a lingering question related to manufacturer supplied dimensions that perhaps some of you have already considered.The New Japan Radio TO-252-3-L1 (DPAK) footprinthttps://www.njr.com/electronic_device/package/TO-252-3-L1-E.htmldoes not directly specify the overall length of the component, from the tip of the two leads to the end of the thermal pad, but rather specifies three separate, individually toleranced dimensions for the lead length, body length, and protrusion of the thermal tab beyond the epoxy body. In order to come up with a single dimension and tolerance to enter into the footprint calculator for a situation like this, I usually add the three separate mean dimensions and then add the square root of the sum of the squares of the tolerances to provide some sort of "statistically OK" measure of expected size and expected tolerance.However, I could see that it may be more appropriate to add up all of the maximum dimensions (i.e. dimension plus positive tolerance) and then add up all of the minimum dimensions (dimension minus negative tolerance) and then determine a new mean and tolerance from these two new maximum material and minimum material sums.What strikes me as incorrect is that most of the time, the extremes are not often reached, so the tolerances become inordinately large, statistically overstated when they are simply added together. Further, it's not like we're fitting a piston into an engine block where it has to always have clearance - the PCB footprint will be larger than the maximum size of the part to make a proper heel or toe fillet, so there is some slop inherent to the process, and the goal is to make the best fit statistically.Any ideas as to the best way I could come up with these composite dimensions? In the past, I've resorted to measuring the actual components as a verification, but that suffers from sampling problems, and also using other vendors dimensions, which might be grossly inaccurate.Thanks!

author: ANTALIFE
author_rank: Frequent Contributor
timestamp: August 11, 2021, 11:40:09 pm
content: The footprint calculators/generators that I have used have the option to deal with mean +/- tolerance OR min & max. With the one you are using, do you have the option to just type in the min & max values?Also I think safest bet is to follow the dimensions the manufacturer has given you (as in work with min & max regardless if they seem too large), that way you will be covered when you do run into an oddly large package

author: free_electron
author_rank: Super Contributor
timestamp: August 12, 2021, 12:08:30 am
content: DPAK is a TO-252 which is standard. Why do you design 300 flavors of a dpak ? dpak is dpak, irrespective of manufacturers

author: montemcguire
author_rank: Regular Contributor
timestamp: August 12, 2021, 12:23:19 am
content: Quote from: free_electron on August 12, 2021, 12:08:30 amThere are some slight variations, but yes, DPAK is DPAK. Currently, I'm using zero DPAK parts, and this is the first, so I want to tune it to the one I'm actually using. NJR for example takes some liberties with their SO8 packages, so I feel that it makes sense to tune their DPAK to what I'm actually placing - not gonna place anything but this one DPAK and they (poorly) specify it.Still, thanks for the reply - a standard DPAK is where I'm leaning, but honestly, the NJR drawings are a little "off", so I want to lean on the NJR specs more than the JEDEC standard that NJR seems to take liberties with. This issue of composite dimensions has come up before, so I thought I'd ask the group to see what the consensus is on how to combine several dimensions into one dimension that is not explicitly defined.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 12, 2021, 01:19:22 am
content: If they don't give a cumulative tolerance, you have to assume the worst -- add them all up, then add toe fillet and that's your pad dimension.In practice, real devices are never as bad as these old crusty drawings. Unfortunately, no one admits whether they're using a more typical package or not.I suppose at best, you take some trust in the footprint they give, which is usually a high-density (minimal size) footprint -- which as often as not, violates their own drawings when IPC clearances are included -- and instead calculate backwards to see what their real dimensions are.But you also don't have any guarantee in doing so.In the end, nothing really matters until the component hits the board. At that point, you see whether it grossly fits or not, pins on soldermask, adequate fillets, and how well they solder. Unfortunately, that's too late, and now you have your assembler notifying you that your build cost is going up because they have to hand rework a bunch of parts or etc... But, if it mostly works, at least you can get some quick feedback, fix it in the next run, and production yields are good....And then the part changes source, to a manufacturer that uses a different part, and production yields fall...On the upside, it's mainly a production thing. Oversized pads are safe, in that no one's going to complain about having extra solder, or soldering area, on the part. (Well, not so nice to have excess underneath a component body, but outside is fine.) It may be helpful for hand rework (enough area to get a soldering iron in there). And if you're doing a small run by hand anyway, you're going to adjust parts and add solder as needed; you might not even use paste. So, don't worry about it too much.Anyway, the proper way is to take the worst case dimensions, add them up, add fillets, and so on. IPC-7351 is a good starting point. It's not too dense reading or anything, and the calculation is basically this simple. Sometimes the result is reasonable, sometimes you get some pretty gross proportions (SMA / DO-214AC and friends are pretty ridiculous) and either just live with it, or decide to trim it because no one seems to be using actual worst-case parts.I will add one thing, don't be afraid to shave pads, like in TSSOP and other fine-pitch parts. MMC dimensions will leave very little if any room for soldermask between pads; check the PCB fab's tolerances and see if it's reasonable to meet it, while keeping pad dimensions reasonable. The trick is, IPC permits side fillet something like -0.03 mm from pin dimension, i.e. the pin is slightly wider than the pad. Gives good results, and understanding this also helps with e.g. SOIC that are just wide enough to get traces between pads.Tim

author: David Hess
author_rank: Super Contributor
timestamp: August 12, 2021, 01:52:38 am
content: When I make my own pad layouts, I accumulate the tolerances toward maximum pad size up to the point where clearance rules would be violated.