FPGA-DAC PCB Design

Question

Hi, I' m using Cyclone III FPGA (EP3C16Q240) and DAC5675A from TI to build an Arbitrary Waveform Generator. I' m currently designing the PCB that has to be limited to 2 layers and I have a few problems I would like to share with you:

1) The split Ground Plane thing. I know I have to separate analog signals from digital ones, I' ve studied some books about it and also googled some, but I have come up with two opinions rather than one. Some people say that the Ground Plane should be separated to an analog and a digital part (and that's also what my instructor told me to do). In this way separate power supplies for the analog and the digital circuits should also be used. Others say that it is better if the analog and the digital signals are just running across separate areas, using a common Ground Plane and they also claim that a split Ground Plane causes a lot of signal integrity problems instead of solving them. Do you have any suggestions on this based on your experience with PCB design/test?

Furthermore, something I don' t understand, is in case I use a split Plane whether I need to connect the two Ground Plane areas (analog and digital) "to a single point preferably close to the power supplies". If separate power supplies are used for analog and digital parts ,do the two areas have to connect together due to signal return paths OR in order to avoid the forming of antennas and, thus, noise?

2) The FPGA PLL power supply. Altera says that the analog PLL circuit should be powered separately using power islands that are isolated by the rest of the Ground/Power Planes. Since I am using a 2 layer board, I dont think it is possible to use such islands and I intend to use regular (digital) 2.5 V power supply for the PLL's. I use one of the device PLL' s along with LVDS SERDES to generate the signals for the DAC running at 400 MHz. Is it possible that I will experience any functional problems due to the PLL power supply?

Thank you in advance

Lambros

altera_forum · Answer

You may start a religion war on the analog/digital plane separation by bringing this issue ;)

The inportant thing when you have digital and analog parts on the board is that they don't share power or signal lines. The power lines include of course the voltage supply, but also the return currents in the ground plane. One way to ensure that (and the easiest way) is to use separate ground planes. Another way is component placement. With the latter method you need to regroup the digital and analog parts on designated areas, but you still need to be careful with the return currents. If you place the digital part between the analog one and the power supply, you can end up with ground noise.

My personal experience is that you get better EMC by using a single ground plane for everything. Having two planes can increase the risk of having voltage differences between the two planes at some frequencies, causing signal integrity and EMC problems. Whith a carefully designed board you won't have more ground noise that with two planes, but if you work with "old school" routers or designers, it can be difficult to convince them ;)

As for the PLL power supply, I think having a separate ground plane is overkill. Altera doesn't even do that on their development kits IIRC. Just keep in mind to put proper filters and decoupling on the PLL supply pins to avoid noise problems with the rest of the 2.5V supply rail.

altera_forum · Answer

Hi Daixiwen and thanks for your reply.

Seems like I m gonna do separated ground planes and use some extra capacitors for the PLL power pins. Another thing that is not clear is whether to connect AGND and GND pins of mixed-signaled IC's to the same (analog) part of the ground plane or to their corresponding ground planes. Any suggestions on that? Finally should I connect the two separated planes at a common point or can I let them completely separated if I use separated Power jacks for each?

thanks a lot,

Lambros

altera_forum · Answer

Usually the datasheet of the chip says how to connect the ground pins. You should connect them to the corresponding ground plane, analog or digital. The two grounds need to be connected in one point.

If you have only one mixed-signal chip, the best is to connect the two planes as close to the chip as possible (under it, if possible). If you have several then it is a bit more delicate.

In an ideal world, it wouldn't matter where the two planes are connected. But if for any reason there is a current leaking from one part to another (either because by mistake a AGND pin is connected to a digital ground, a DGND pin to the analog ground, or because of a design problem inside the chip) you can have return current problems. As an example if you have a current from the digital power supply that somewhat ends up partially on the AGND plane, it will try to find its way back to a decoupling capacitor on the digital part. It will go through the AGND plane, the AGND-to-DGND connection, and in the DGND plane to the capacitor. If the AGND-to-DGND connection is just under the chip it wan't matter a lot, because the current will follow a short path. But if the connection is on the other side of the PCB, this current will catch/generate a lot of noise on its way. So if you have several mixed signal ICs, try to keep them as close as possible and connect the two planes between them.

altera_forum · Answer

Daixiwen, thank you very much for your help. I guess there aren't many people who actually construct their boards for themselves these days. :)

altera_forum · Answer

To point out my position in this religion war: The concept of split planes is mainly an erroneous belief. Most designs are better with a continuous common plane respectively multiple stacked planes. You have to isolate sources of interfering currents, that can spread over the ground plane. In some cases, separated ground isles respectively local power plane areas can help, e.g. for SMPS functions. In- and outbound nodes are then bypassed against this local ground. Most digital and mixed signal devices are injecting common mode currents into the ground plane, they also cross the analog/digital boundary. With separate or split planes, these interfering currents can cause higher interference voltages on the board, you get possibly additional structural resonances and so on. The only convincing split plane designs I've seen are development kits, involving a single mixed signal device, e.g. an ADC. Unfortunately most real world designs can't follow this trivial topology.  The situation is different, if you leave the mixed signal region and go to low-level preamplifiers, output filters and similar functions for pure analog signals. They better reside on separate boards or possibly on an isolated region of a main board. But implementing well considered grounding schemes or even better, differential analog signaling, they can coexist with mixed signal design parts without problems.  Regarding the specific questions: - A two layer PCB won't achieve a continuous ground plane, nor realize an ideal split plane concept. It's a compromise in everything. Practically, the ground will be split at the DAC position, so you can declare it as an implementation of whatever concept you prefer... Even on a two layer board, you should be able to implement effective bypass caps.  - With Cyclone III, PLL issues have been considerably reduced by the internal VCCA regulators. Practically, local filtering of each PLL supply with multiple bypass caps and a ferrite bead or series resistor is the only option achievable with a two layer PCB. Strictly spoken, unused PLLs won't need this filtering. - I expect, that SNR of your generator mainly depends on a good differential output amplifier design.

Forum Discussion

FPGA-DAC PCB Design

8 Replies

Recent Discussions

Arria 10: Remote Update Watchdog unpredicted behavior

Cyclone IV E(EP4CE30) FPGA JTAG and USB-Blaster

Agilex 5 BSDL Files

Timing Behavior of Remote Update IP After Reset on Cyclone 10 GX (10CX150YF672E5G)

Agilex 7 R-Tile RBES FPGA – Board Fails to Power On and JTAG Not Detected