PCB size  vs. total component footprint size - Page 1
Forum section: electronics / projects

author: halexa
author_rank: Regular Contributor
timestamp: January 05, 2015, 02:46:10 pm
content: Hi,Are there any golden rules for how large PCB you gonna need if you know the total footprint size of the components your gonna use.In my case my PCB is 4154mm2 and i calculated the total component footprint to be 2300mm2. And it's a four layer board.

author: tszaboo
author_rank: Super Contributor
timestamp: January 05, 2015, 02:51:47 pm
content: I dont think I ever made that calculation, because there are several factors effecting this. Just compare a QFN with thermal pad and a DIP package. For the same size one occupies two layers just for the component, while the other basically nothing.Maybe there is a rule, but I woul look at the PCB editor, and estimate.Nevertheless, I suspect that you need to go to double component side.

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: January 05, 2015, 04:11:13 pm
content: No golden rules. More like wooden, or styrofoam maybe.It's all dependent on your design rules. This includes things like via in pad, assembly house, testability, silkscreen, etc.First you need to include the assembly clearance around each part. You can't just shove parts arbitrarily close together.Then you need to include the board keepin, you can't place parts too close to the edge. There's also the pullback you need to include for the ground plane, you should not route traces close to the edge, you should have enough copper underneath.Each res/cap might need a via or two, include that in your surface calculations. Then add in the netlist info, how many power and ground pins do you have? Add those vias as well.The rest is like a gut feeling depending on the design. Is it capacitor bound? Is it I/O bound? Component bound? Connection bound? Etc..For example, I had a customer that absolutely wanted a silkscreen refdes for each part. On a large DSP board with lots of parts. You needed board space just for that. They didn't care but you still needed to think about that.Then just toss everything in the PCB software and play around.

author: halexa
author_rank: Regular Contributor
timestamp: January 05, 2015, 04:27:56 pm
content: Yeah I understand there are allot of variables in play. Think I need to do the PCB footprint for my bigger components and lay them out on the PCB so I get a visual feeling of the size taken.Reason I ask is that our customer are providing the PCB housing and the system specification, and I want to on an early stage pull the brake if the housing is to small.

author: tszaboo
author_rank: Super Contributor
timestamp: January 05, 2015, 04:37:36 pm
content: You dont have the footprints ?Consider different density footprint:http://blogs.mentor.com/tom-hausherr/blog/2011/01/28/pcb-design-perfection-starts-in-the-cad-library-part-12/

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: January 05, 2015, 04:50:03 pm
content: Quote from: halexa on January 05, 2015, 04:27:56 pmNow is the time! You need the netlist info, like footprints and # of connections. Any length matching required? Like a DDR3?Also four layers could mean one solid ground plane, but only power islands on the inner layer with space for routes as well. YMMV, etc.Or you can do a hybrid HDI design, which I do a lot. If you have a part with many power nets but few IOs, like an ADC let's say, I put all the power on the outside and route inside, but not for all chips.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 05, 2015, 08:32:58 pm
content: It's pretty hard to do a layout with total board area under twice the total footprint area (assuming double side load and standard width and space rules).Generally, you start to need expensive things like finer than standard width/clearance/annulus rules, and blind/micro/lasered/plugged/filled/solid vias (which are acceptable for via-in-pad), to push as low as equal area (or even less, sometimes -- 3D shape allowing). For ideas, look at any microelectronics these days: cell phones, tablets, laptops, etc.If you need a low cost fab (4 or 2 layers?) and lots of special traces (characteristic impedance, length matching, high shielding, high power or high dissipation), expect to need more area to reserve for routing and stuff.So yeah, double isn't bad, seems reasonable to me offhand. Figure more or less depending on required fab cost, lead time (how much time you have to screw with it..) and so on.Tim

author: tszaboo
author_rank: Super Contributor
timestamp: January 05, 2015, 10:45:45 pm
content: Quote from: T3sl4co1l on January 05, 2015, 08:32:58 pmI would rather consider making a sandwich with board to board connector, if there is space for it. For smaller quantities that yields lower total cost than going crazy with the technology.If price wouldnt matter, I would go crazy with flat-flex, HDI, plugged microvias ...

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 06, 2015, 08:17:01 am
content: Yeah, if you need small outline but not low-profile, you can nearly double the available layout area by stacking just one board -- something impossible to achieve in multilayer, regardless of the layer count.Multiple boards require more connectors (unless you use a stacking type with long connecting pins -- if a common bus is acceptable), or a backplane, both of which cost more outline, but as long as the remaining board areas are a net gain, no problems.Such design does force your individual boards to be low profile (or to have conspicuous cutouts for bulky components -- and to manage and synchronize those features very carefully between the boards as the design evolves!), but that shouldn't be a big or insurmountable problem. For example, tall capacitors can be split into multiple parts in parallel; on a powerful supply, you could do worse than dedicate an entire card to filter capacitors, for instance.I have heard opposition to multiple boards in a design. Managers assume it increases development and production cost. Personally, I don't see how. But whatever.Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 06, 2015, 08:38:13 am
content: Well, you can always hang the toroidoff the sideif it's hand wound, or find a vertical type if it's purchased. Big magnetics will always be big. If your circuit isn't doing much, maybe you should consider a higher performance controller...Tim