128-TQFP Footprint  - Page 1
Forum section: electronics / general

author: AndrewHodgson
author_rank: Contributor
timestamp: May 23, 2022, 10:04:35 am
content: Hi,I'm trying to do a footprint for a 128-TQFP component, but I'm struggling, does anyone know where I can find some good recommendations?If found a Renesas footprint but I was curious about the solder resist information too. I presume I want some resist between the adjacent pads but I'm not sure how much. It's a very fine pitch component (0.4mm). The pad size of 0.2mm also seem a bit thin, other documents seem to recommend something larger like 0.25mm with a 0.05mm resist window.I assume having no resist between adjacent pins is a bad idea?Does anyone know where I can find a good reference document? Which IPC standard is relevant?Thanks in advance.

author: jpanhalt
author_rank: Super Contributor
timestamp: May 23, 2022, 10:38:13 am
content: Check the manufacturer's datasheet. It is either there or in a compendium of the footprints it uses.

author: voltsandjolts
author_rank: Unknown
timestamp: May 23, 2022, 12:21:24 pm
content: My world would be a simpler place if there was only one TQFP128 footprint!Not sure that soldermask between pads is worth bothering with, but check your pcb manufacturer for their min mask width specs.e.g.eurocircuitsis 0.075mmWhat is the part and which cad are you using?

author: AndrewHodgson
author_rank: Contributor
timestamp: May 23, 2022, 01:11:11 pm
content: I'm using CADSTAR. I was hoping there would be a formula that exists for calculating standard footprint sizes when the footprint doesn't appear to be available.I think possibly the footprint is difficult to find because the package dimensions are basically identical to PQFP and you can just use that as a reference for a footprint?The min mask width spec seems ok for what I've done. I think 100um to 75um is fairly typical.Thanks

author: eugene
author_rank: Frequent Contributor
timestamp: May 23, 2022, 02:54:39 pm
content: I use 0.25mm wide pads with 0.4mm pitch TQFP with no mask between pads. Check with your PCB fabricator. If they can reliably put a sliver of mask between pads it will help reduce solder bridges, but it's not 100% required.

author: free_electron
author_rank: Super Contributor
timestamp: May 23, 2022, 03:11:48 pm
content: It all depends what your board fab can do.You need a 0.075 to 0.1 soldermask dam. Anything smaller than that risks peeling during handling. You need a 0.05 mask to solder clearance. So on a 0.4mm pitch part that leaves you with 0.2mm copper for the pin. ( assuming a 0.1 sliver.) If you go with a 0.075 dam you get 0.225mm pad )is this really a qfp or is it a qfn ? in case of a qfn i strip the slivers . you want the center pad to be able to outgass correctly.

author: AndrewHodgson
author_rank: Contributor
timestamp: May 23, 2022, 03:48:56 pm
content: It's TQFP. I've opted for a 0.25 pad, 50um resist window and 0.75um dam as suggested. I have some room for flexibility on the supplier, but I've also read that you can use two stencils for 0.4mm pitch components. One for the normal components and then a thinner one for the 0.4mm components. This might be a better option.Not sure what you mean when you say you strip the slivers? Does this mean you're not using any resist?Thanks for your help, it's very much appreciated.

author: Feynman
author_rank: Regular Contributor
timestamp: May 24, 2022, 06:14:41 am
content: As others have mentioned the first place to go is the manufacture's datasheet.If you are looking for some sort of formula, relevant standards are IPC-J-STD-001 and IPC-7351.Or you use a third party tool that is kind of based on the IPC standards and adds a few improvements like the tool from pcblibraries.com (they have a free version of their tool).As for solder mask the best way is normally to make solder mask openings 1:1 land size and leave the manufacturer the option to resize openings according to their capabilities (e. g. in the fabrication notes).No solder mask between pads is definitely not recommended. If you have a fine pitch part you should double check with your fabricator, if he is able to leave some solder mask between the pads. Your assembler will thank you