Multiple DACs on board, Digital and Analog grounds - Page 1
Forum section: electronics / projects

author: msngupta
author_rank: Contributor
timestamp: May 02, 2016, 04:31:29 pm
content: Hi,I am a newbie to pcb designing. I am designing a four layer (one dedicated for ground plane and another for power plane) board which has an FPGA and fews 14 bit DACs (AD9744). The DAC has high sampling rate (~200 MSPS) and I am afraid of switching noise coupling to the DAC output. So I wanted to ask if I need to split Analog Ground and Digital Ground?The image attached roughly shows the positions of various IC's.I found few articles about dealing with this problem which provide different solutions and I am confused which on to follow1)http://www.hottconsultants.com/techtips/split-gnd-plane.html2)http://www.ti.com/general/docs/lit/getliterature.tsp?baseLiteratureNumber=slyt4993)http://www.analog.com/library/analogDialogue/archives/46-06/staying_well_grounded.htmlThough this might be an old question, If I follow the prescription given in first article, where one uses only one ground plane but different regions.My doubt is about the power connectors, where do they lie in the diagram specified byhttp://www.hottconsultants.com/techtips/a-d%20gnd%20plane.gif?How should I route the power connections from the connectors to the corresponding ICs (DAC's and OPAMPS) ?Given that I follow proper discipline in routing the digital signals in digital region and analog signals in analog region, Which prescription should I follow and where should I place the power connectors and route the power plane?Any hint will really help.Thanks in advance.

author: nctnico
author_rank: Super Contributor
timestamp: May 02, 2016, 05:23:52 pm
content: I'd put the FPGA on one side of the board and the DACs + analog on the other side of the board. You can use ferrite beads to limit how far HF currents will reach. Remember current always goes in a circle! You can shield the digital section from the analog section and vice versa by putting ferrite beads in the supply lines close to the FPGA and analog chips. Another trick is to use series resistors in the digital lines to the DACs to minimise the HF current which flows between the DACs and the FPGAs. If a signal goes high, current goes out of the FPGA (from a decoupling capacitor) into the digital ground of the DAC and this current needs to flow back into the decoupling capacitor near the FPGA. For a signal going low the same happens with an opposite current.

author: msngupta
author_rank: Contributor
timestamp: May 03, 2016, 06:52:18 am
content: Thanks for you reply,But I still didnt get my answer, should I split the ground plane or not ? If yes how ?I am using the ferrite beads for power lines and series resistors for the digital lines.I cannot shift the location of the FPGA, shifting the FPGA to one side makes the routing of digital lines really painful.

author: Siwastaja
author_rank: Super Contributor
timestamp: May 03, 2016, 08:54:55 am
content: You are not going to get a "correct" answer whether to split the planes or not, because people disagree. Both styles are widely used.I'd say avoid splitting, since it's easier not to split. Just keep physical separation enough, and have all digital traces go in the digital section. This way, return currents in the ground plane also go in the digital section. If you maintain an inch of separation, the amount of return current from digital signals in analog section is miniscule. Adding a split would bring it down to zero, but it would bring in another set of possible problems, and it's not always possible to do a proper split anyway. I.e., where do you join the planes?Butdosplit the supply planes, or use a star-like topology for supplies, with good local bypassing.

author: nihtila
author_rank: Regular Contributor
timestamp: May 04, 2016, 03:53:04 pm
content: Ground separating is a neverending debate. I have been reading Henry Otts book and papers (you can find some articles on Google) and he is strictly against splitting the grounds. The separation should be done with component layout. But then again, when layout is good, splitting the grounds shouldn't do much difference anymore. So I would say lay out the components like there would be a slit but do not make the slit. As have been said, it all comes to paying attention to the return currents.I would arrange the components so that you have analog and digital components on different sides of the board, as was already suggested. That will probably makes the split power plane also easier to implement, and keeps the return currents in their own sections. Also, remember to keep ground plane adjacent to the main routing plane, and power plane adjacent to the less important routing plane. High frequency return current can flow on ground plane or power plane, and slit on a plane (power plane in this case if you keep ground plane solid) forces the current to flow in a longer loop.I found Henry Ott's Electromagnetic Compatibility Engineering a good and practical, relatively easy to read, book to study EMC issues, also related to PCB design.

author: Wobbegong
author_rank: Newbie
timestamp: May 04, 2016, 04:43:32 pm
content: You should definitely not split the planes unless you really know what you are doing, and even then you are still most likely to get the best performance by not splitting the ground planes. Splitting planes= minimal (if any) benefit with a high probability of making your design worse.As others have said, just give the analog stuff its own 'quiet' area of your board and keep the digital stuff away.

author: danadak
author_rank: Super Contributor
timestamp: May 04, 2016, 04:57:43 pm
content: Some application help -https://www.dropbox.com/s/ruaf9booe17jk8n/PCB%20Layout.zip?dl=0Regards, Dana.

author: f5r5e5d
author_rank: Frequent Contributor
timestamp: May 04, 2016, 05:23:29 pm
content: system questions impact layout toowhat digital inputs? internal to case, external? diff, serial, isolated...analog output frequency range, balanced/isolated, to external, or again used internally other boards in one case