PCB design question - Page 1
Forum section: electronics / projects

author: TheRevva
author_rank: Regular Contributor
timestamp: April 18, 2015, 01:10:43 am
content: Hi all,I _hope_ this is the right place to ask... (The sub-forum title does state 'technical stuff'... LOL)I've designed a few (hobbyist) PCBs in my time, but they've ALL been thru-hole projects with simple 100mil (0.1") centers.I've never had to design / assemble anything of an SMD nature (ok, that's not 100% true, I once had to hand solder an 0603 varicap diode into a small stereo LPFM transmitter... UGH!)I'm now toying with a design that uses some SO14, SO28W (0.05"/1.27mm pitch), MSOP8, SSOP16, SSOP28 (0.025"/.65mm pitch) chips along with a handful of 1206 passives.It's quite possible that this board might be 'hand assembled' by SOME constructors (some with a toaster oven, others with a fine tip iron using 'drag soldering'?)I'm after some 'guidelines' as to how densely I can cram the components on the PCB without creating sheer havoc for those wishing to hand assemble it.Things like chip-to-chip spacing, chip-to-passive spacing, pad-to-via spacing (taking into account solder masks etc) are all 'new' to me.If nothing else, it'll be interesting to hear your opinions.

author: moffy
author_rank: Super Contributor
timestamp: April 18, 2015, 01:17:19 am
content: Ugh, sounds horrible. Better you than me, best of luck.

author: RobertHolcombe
author_rank: Frequent Contributor
timestamp: April 18, 2015, 02:05:17 am
content: I perform regular SMD rework on components down to 0805, on boards with minimum chip-to-chip spacing of ~0.5mm, I'm not equipped or required to work on anything smaller. I'd say layout and component clearance is more of a concern for rework than initial assembly - even when hand soldering you can deal with high density layout by being mindful of the order in which you populate a board.

author: Unknown
author_rank: Unknown
timestamp: April 18, 2015, 03:11:46 am
content: Quote from: TheRevva on April 18, 2015, 01:10:43 amI don't think you'll find a set of hard-and-fast rules for something with a bunch of different pitches/sizes and two totally different assembly methods.My general rule of thumb is to use the reflow dimensions for pads (since that's critical for obtaining a good reflowed joint), and space/orient parts to leave enough room to get a reasonably large iron tip in without touching other components/pads/vias. Defining "enough room" is the key though, and depends a lot on the assembler's skill & equipment.Example: I use mostly 0.65mm/0.5mm pitch semis, 1206/0805 passives, & hand-soldered. Until now I've never taken care to actually measure spacings when laying out, but just eyeballed it from experience. Turns out that I typically use 1.5mm between pads of components in-line, and 2.25mm between centres of components side-by-side. That gives plenty of room to get a 1.2mm or even 1.6mm tip in there for soldering.Some would argue that's way too much space - and I'd tend to agree, but it makes for easy hand-assembly and you don't have to worry so much about the order of population (which can be a pain if you want to test sections as you go). If space is tight I'll sometimes squeeze down to 0.5mm between pads end-to-end, or 2mm between centres side-by-side, but I try not to make a habit of it.

author: alank2
author_rank: Super Contributor
timestamp: April 18, 2015, 03:36:42 am
content: What are you using for a pcb layout package?One nice tool someone pointed me to here lately is the pcb library expert. It can generated packages for you that you can import into your pcb package. I always use the "most" density level.I've done a couple of smd boards and I still tend to stick with a 0.025" grid even though many smd pads no longer align to it.

author: mrpackethead
author_rank: Super Contributor
timestamp: April 18, 2015, 06:10:55 am
content: i work with .4mm pitch and 0402 by hand. I do have to do the smaller stuff under magnification. And thats just with a standardish ( Hakko FX-951 ) iron. Really it comes down to practice, and technique. Give it a go and try, you'll be surprised what you can achieve. A toaster oven solution is only as good as the solder paste that goes on btw, so while it speeds things up, it doesn't help much in terms of precision.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 18, 2015, 06:12:05 am
content: I normally make pads a tad longer than IPC recommendations (which are usually -0.03/+0.1 mm side fillet, +0.35 mm heel and toe fillets over worst-case dimensions). So SMD chip and leaded (SOIC, etc.) pads might be 0.5 to 0.8mm longer than they need to be, to allow some extra room for the iron's tip.DFN/QFN still have an outer fillet that can be hand soldered, and would benefit from extra length in that case; but the heel and side fillets are nonexistent (+/- 0.1 mm or something like that, no expansion/draft) because they're directly sandwiched by the part. Other leadless style parts (LGA, BGA..) simply use net-size pads and that's that.Component spacing is usually recommended something like 50 mil (1.2 mm) between bodies. Enough space to get tweezers and an iron in there. More for leadless parts that need hot air, and more around tall components that are hard to get in around (say if you have SMTs laying around a big electrolytic capacitor, or connectors/headers).For automated assembly, you should also reserve space (several mm) around through-hole pads that are to be wave soldered. Usually what they'll do is, assemble and reflow the top and side SMDs in two steps (using glue as necessary), then insert THT components and use either complete wave or selective wave soldering. If the reflowed SMTs can't be exposed to wave (e.g., they'll float right off..), a guard jig is needed, and it takes some clearance (a conical opening around the pins to be soldered) to do that. So, tall SMTs have to be further away than short SMTs to land outside of that cone.For hand soldering, this clearance isn't such a big deal, but use some common sense when placing SMTs near THT pads. Provide a clear path where the iron can be laid down alongside the row of pins, for effective soldering.Tim

author: TheRevva
author_rank: Regular Contributor
timestamp: April 18, 2015, 10:51:04 am
content: @Alank2:To answer your question, I mostly use Eagle although I've done a few with Kicad.BTW, you're a little RIPPER!!!I had been wasting FAR too much time trying to layout the SSOP packages on a 0.325mm metric grid (i.e. 1/2 of the pin pitch) and then trying to 'make them connect with other, imperial components.Now that I've restarted it all using a strict 25mil grid throughout, it went MUCH better... (I had to be a little careful with the SSOP28 package though since the errors accumulate)THANX!@Felix-The-CatI completely understand that there's no 'rules' (which is why I only asked for 'guidelines').The guidelines that you've mentioned though seem quite reasonable.I'm going to use 75mil (1.905mm) where you use 1.5mm and 100mil (2.54mm) where you use 2.25mm.(Being a little larger should 'help' old farts like me who are a bit 'shaky'... LOL)

author: tggzzz
author_rank: Super Contributor
timestamp: April 18, 2015, 07:45:36 pm
content: Quote from: TheRevva on April 18, 2015, 01:10:43 amI thought that would be difficult/impossible at home, but I was pleased to find it is all very do-able at home.Seehttps://entertaininghacks.wordpress.com/2015/03/25/creating-pcbs-with-surface-mount-components/and the linked pages for my experiences.

author: marshallh
author_rank: Unknown
timestamp: April 18, 2015, 09:13:44 pm
content: Just make some boards, make notes as you assemble them.Things like:1. Don't let SMD parts share pads2. Avoid placing small passives next to large connectors3. If hand soldering, orient all passives the same way to minimize effort4. Leave enough space on the sides of QFP/SOICs to lay wick on the leads5. For easier soldering og QFN/qfps, lengthen the pads outwards by 25%After switching to 100% reflow prototyping with 0402s, 0.8mm bga and qfn, I wouldn't do it any other way.

author: kjs
author_rank: Regular Contributor
timestamp: April 19, 2015, 03:48:55 am
content: I solder 0201's and 0402's most of the time with 0.35 to 0.5 pitch IC's next to them. Some with the pretty large IPC rules but often with smaller pads. You have to follow a sequence (low profile to high profile) and the board shouldn't be to tightly packed. all done with a Metcal and a fine tip. If it gets to tightly packed it's stencil and solder paste then hot-plate or vapour phase. Only for MLF/QLF type packages we changed the layout to make the pads come a bit further outside the package. Otherwise it's a bit difficult to heat up the pad with the iron.However, my eyes are getting older and I have to use a stereo microscope to do that.It's all a matter of technique and practice, practice, practice........

author: TheRevva
author_rank: Regular Contributor
timestamp: April 20, 2015, 04:13:02 am
content: @MarshallH:Hmmm, I had not considered the (obvious?) need to be able to 'wick' the solder, whether to 'fix' a solder bridge (which is more likely on the 'prototype' soldermaks) or perhaps to recover and / or replace a component entirely.Thankfully, I had already came up with all your other suggestions. I guess I that means I _DO_ possess some degree of common sense after all (despite what I am constantly told.... LOL)@KJS:While I completely agree on the 'shouldn't be too tightly packed' guideline, I was trying to put a number on it. Felix gave me a 'starting point' and I'm going to go even MORE sparse since I'm somewhat of an SMD noob!@tgggggggggzzzzzz:I'll take a look @ DesignSpark sometime. I 'toyed' with KiCad for a while mostly because of the 3D view capabilities that I don't have within Eagle 6.4.0. It'll be _interesting_ to see how 'complete' the DesignSpark 3D models are...(I could argue that a 3D view is almost in the 'optional bells and whistles' category, but that doesn't mean I don't WANT it... LOL)OMG!!! I just installed it and 'imported' my design as it stands direct from Eagle and... I IMMEDIATELY get a decent 3D view... IMPRESSED!!!!Sure, the silkscreen needed some 'touchups', and a couple of components have obviously incomplete 3D models, but overall I am impressed so far.

author: tonyarkles
author_rank: Regular Contributor
timestamp: April 20, 2015, 06:04:07 pm
content: Yeah, for hand assembled boards with fine pitch SMD, by far the most important thing I've found is to make sure there's enough room around the ICs to be able to sneak a piece of wick in to clean up any bridged pins.I've got a board open in Eagle that has an array of SOT23-5 chips with 0603s in between them. It looks like there's ~0.625mm spacing between the pads and it was no problem to rework with a fine tipped iron. The 0603 pads are a bit bigger than the components that go on them, so that adds a bit more clearance.