I am trying to use a Nichicon UMA1V2R2MCD2 (Mouser 647-UMA1V2R2MCD2) 2.2 µF, 20%, 35 V dc, Aluminum electrolytic, radial leaded, capacitor. The lead spacing is very narrow at 1 mm ±0.3 mm and lead diameter of 0.4 mm. Mouser is now using an outfit called SamacSys (a British company) for graphic symbols, land patterns/footprints, and 3D renditions. I downloaded their file and found the footprint had overlapping pads. I wrote an e-mail to them and they changed their footprint but the pads still touch. I wrote another e-mail to SamacSys but have not had a reply.
How do I do a proper footprint? One way I see is to place the plated through hole pads further apart. This would be okay for hand insertion but machine insertion would be a problem. Another way would be to place the pads so that there is no copper on the side facing the other pad. Any suggestions or insights?
–Thanks, Larry
Just go to the Mouser website and enter the Mouser part number of 647-UMA1V2R2MCD2. This will take you to the part screen where you can click on the PDF datasheet icon that will open the Nichicon datasheet for the part.
–Larry
What about pads with drill 0.3mm and X-size 0.7mm?
Then speak to yourr manufacturer to check if there is enough ring. There is still a 0.3mm clearance, so try even 0.75mm X-size.
A Forum member who expects a timely reply will demonstrate respect for other users by including a Datasheet Link , a polite member who has been raised properly will attach the datasheet e-uma-1218975.pdf (142.8 KB) and the supplicant who gets the most attention will include a relevant, legible, sketch or illustration.
It looks like this component is just barely compatible with current practices for inexpensive, quick-turn boards. (Ref: Seeedstudio “PCB Design for Manufacture”, v1.1 )
Start with hole size for the component leads of 0.5mm (20 mils) diameter - and hope that manufacturing doesn’t complain that ths is too small. The pad around this hole must have an annular ring of 0.15mm (6 mils) or more. That leaves 0.2mm (8 mils) of spacing between the two pads. These values meet the minimum requirements for several (but not all) board fabricators.
I’ve used the UMA series caps in a few designs, but I remeber they were tough little buggers to solder. I guess thats what you get when you want subminiature… I will see if I can find the footprints, but I remember modifying a standard footprint. Make the pads oval so you have some more area to put your iron on.
My favourite low cost board maker can do 0.3mm holes, so a 0.5mm drill hole is easy enough, but you will need a oval or offset pad to get a chance of a good joint
I was thinking that a 0.4mm lead in a 0.5mm hole is just barely usable for populating and soldering a PCB assembly - especially when tolerances result in fatter leads or narrower holes.
You and @Jules are correct that an offset oval (or rounded rectangle) pad will make manual soldering and rework much easier.
I am assuming manual insertion. Through hole auto insertion requires bigger holes.
The other parameter that you don’t see in the basic capabilities lists is hole to hole spacing. At these sizes there is a real risk of the hole breaking out.
You might be better off with 0.6mm holes, but increase the pitch to 1.2mm.
I guess these parts are a lower cost alternative to small tantalums.
2000 hours endurance at 85C is a heavy price to pay though
For essentially the same cost you could use a ceramic capacitor: Murata GRM188R6YA225MA12D
The ceramic cap has better electrical performance, although some applications depend on the series resistance of electrolytic capacitors to dampen resonances.
For that supplier, that works out as 0.3mm side of hole to side of hole, so 0.9mm centre to centre for 0.6mm holes. That means 1.0mm pitch/0.6mm dia is just OK
For all of those that have replied to my posting–a hearty thank you. The suggestions and documentation/resources are well received.
To: pedro–what is meant by “X-size”?
To: Dale (dchisholm)–yes, I have been thoroughly chastised, I’ll do better in the future. I will need to relearn the use of snippets. How did you get the red line around the info in your snippet? I have also seen yellow coloring used and wonder how that is done?
This PCB is for audio frequencies at room temperature with all parts of THT and will be hand inserted and hand soldered.
I am having a go around with Ultra Librarian and SamacSys about this part, both about the graphic symbol and especially about the land pattern/footprint.
–Regards, Larry
ShareX seems to have that feature, too. ShareX is a bit complicated tool, but has everything you might ever need, including simple screencast feature (everybody who writes here or reports bugs should learn how to record screencasts!).
