What to do with the bottom layer? - Page 1
Forum section: electronics / beginners

author: beastmanrage
author_rank: Newbie
timestamp: November 10, 2012, 09:05:22 am
content: Hi guys,So I'm designing a "one-off" for a school project and decided on a 4 layer approach:SIGGND3.3VNADAI actually had no need for the bottom layer, do you guys recommend a ground pour or something special?Note: I only have a i2c bus (400 KHz) and 4 analog lines that all feed into a microcontroller for A/D.Thanks,Paul

author: PSR B1257
author_rank: Frequent Contributor
timestamp: November 10, 2012, 09:17:22 am
content: 4 layer for a school project-PCB ... ambitious.I cant imagine, you really need that.Can you post the schematic of the circuit?

author: beastmanrage
author_rank: Newbie
timestamp: November 10, 2012, 10:02:26 am
content: Hi PSR B1257,I initially had a 2 layer design. I decided to go 4 layer to reduce possibility of EMI. This is a time-sensitive "one-off", so I figured I'd trade some cost for confidence.Also, form factor is a huge constraint for me. Fitting 5 devices on a 30mm X 35mm is not allowing me much routing space. Ridding of the 3.3V route definitely opened up some space, but I still have this bottom layer with nothing on it.I would assume a simple GND pour would be fine, but I don't want to be wrong and create some large antenna.If I have multiple ground vias throughout my design, would pouring a ground plane on the bottom layer act somewhat like a "faraday cage" for the power plane?

author: SeanB
author_rank: Super Contributor
timestamp: November 10, 2012, 11:12:13 am
content: Use the bottom layer as ground, and whenever you have a via to the inner gnd plane make it a through via and connect the 2 planes. stitch them at the edges of the board and add an extra via or two wherever you have decoupling capacitors. Make all the 3V3 vias non blind and have a clearance about each on the ground plane as well, you can also bring test points out with Vias to the back so you can easily do probing without worries.

author: ivan747
author_rank: Super Contributor
timestamp: November 10, 2012, 11:24:11 am
content: Quote from: beastmanrage on November 10, 2012, 10:02:26 amNote that 4 layer boards usually take more time to manufacture and are harder to inspect.

author: ivan747
author_rank: Super Contributor
timestamp: November 10, 2012, 11:27:55 am
content: And yes, having ground and 3v3 sandwiched across 3 layers acts like a capacitor.Since the board is very small, I think you don't have to worry about the I2C lines getting capacitance the ground layer.

author: Smokey
author_rank: Super Contributor
timestamp: November 12, 2012, 04:48:13 am
content: Don't let people scare you off of 4 layers. The only real drawback is board cost. As long as you are getting them from a reputable board house with etest, you shouldn't have to worry too much about inspection. Advanced circuits has really good student deals for 1-off boards, 2 and 4 layer. They will let you order just one PCB and the lead times are crazy fast assuming you are getting standard spec boards. Quality is always top. Give them a call and talk to a rep. They are always super helpful.Since I haven't seen what your schematic/layout looks like and assuming it's not already done, as far as what to do with the 4th layer I'd say route signal traces on it along with the top signal layer. Since it's a 1-off and you don't have to worry about assembly cost you can put components on both sides. That certainly makes the layout easier.If you go with double ground planes because the other one isn't continuous enough or something, make sure you stitch a bunch of vias connecting them together wherever you can. Don't leave big open spaces with no vias connecting the planes if you can avoid it.

author: westfw
author_rank: Super Contributor
timestamp: November 12, 2012, 05:50:30 am
content: If there's really nothing on the bottom layer, I'd put down some "spare" footprints in case you need a hardware patch. And enough vias to connect important signals from the top layer...

author: w2aew
author_rank: Super Contributor
timestamp: November 12, 2012, 03:16:16 pm
content: If you REALLY want to EMI-proof your design, you can use the top and bottom as ground, and bury your SIG layer. With lots of via-stitching of the grounds, makes for a very RF-robust design. However, debugging, modifications, etc. will be very difficult if your signal traces are all buried of course! ;-)

author: Smokey
author_rank: Super Contributor
timestamp: November 12, 2012, 06:43:02 pm
content: One trick if you are going to bury all the signal traces on an inner layer and have a lot of routing space is to make all the connections to IC pins coming from outside the chip. Try not to bring the trace connections up under the chip. If all the traces are coming into the outside of the pads then you can cut and jumper without having to lift the pins or remove the chip.Since you said you are feeding some analog lines into the micro, you can also have separate analog and digital ground planes that are single point connected. I usually just do an analog ground plane island in the middle of the digital ground plane layer if it's not that big.

author: Neilm
author_rank: Super Contributor
timestamp: November 12, 2012, 07:51:21 pm
content: Quote from: Smokey on November 12, 2012, 06:43:02 pmI have found better results just having a one ground plane on a board rather than separate digital / analogue grounds on a 4 layer board. This is due to inevitably having a signal referenced to one going into a chip supplied from the other. If you follow the current flow, you can find it wandering all over the board.Neil