PCB Layout 常见问题
Grounding Techniques
FAQ: Should I be concerned with layout if the converter is only 16-bit?
A: A great circuit design can be ruined with a poor layout. So even with a 12-bit system layout can be critical. Obviously with even higher resolution converters the layout becomes even more critical. One of the layout pitfalls include mixing of digital and analog signals where they can cross each other and increases noise. Another is poor grounding where noise can be picked up through a ground trace, or where return currents are forced into a noisy area of the board.
FAQ: Where do I connect Analog and Digital grounds?
A: Most all data converters require that the Analog (AGND) and Digital (DGND) ground be no more than 0.3V apart. This is generally shown in the Absolute Maximum specifications in the datasheet. To effectively achieve this requirement, there must be a low impedance path between the two grounds at the data converter.
The most effective method of doing this is to use a single ground plane and connect AGND and DGND directly to the plane as close as possible to the ground pins of the converter. If split ground planes are used, connect the ground of each plane together under the converter with a copper connection as large as possible to reduce overall impedance.
Consider using ground planes versus ground traces, and if possible a single ground plane versus split ground planes.
Here are some data converter grounding examples.
FAQ: I don't need a ground plane do I?
A: A ground plane is best because it provides the lowest impedance for the return current path.
Q: As long as the grounds are all connected, why does it matter?
A: From a schematic point of view, all the grounds just connect to a symbol(s) and is basically a reference point. A simulation of the schematic places the ground symbol at a specific node. Usually that node is 0V. In reality it is quite different. If you take a good look at a finished 2-layer PCB, from the edge side you see two copper layers separated by some form of dielectric material (usually FR4.) This is one form of capacitance on the PCB. Any trace will have material characteristics which will impede electron flow (resistance) and have some value of inductance. This is also true for any holes or vias on the PCB. So the difference between the schematic and the PCB is that a real value of impedance exists between any two ground connection points.
Q: If I use thick traces, won't that be good enough?
A: Maybe, but usually doubtful for high resolution analog-to-digital converters (ADC). This is primarily due to noise. The noise can be a result of poor return current paths, or from noise pick up on the ground traces from external sources. Some external sources of noise can be a result of EMI/RFI, or AC power lines. Often times ground traces will act like an antenna and pick up the stray radiated noise (like from a cellular phone.) Trace inductance can be a real threat to damaging the data converter from short term events like ESD.
Q: My PCB is 2-layer, and I don't have enough space for a ground plane. What problems can I expect?
A: With an ADC, the noise will affect performance. You will see a much larger than expected code variation between conversion results. A 24-bit converter can easily lose half the resolution due to noise. If you suffer from noise, take a long hard look at your overall layout. Try to utilize as much ground area as possible on both sides of the board.
FAQ: Which is better a single ground plane or a split ground plane?
A: This is rather difficult to answer. There are many viewpoints on this, so every PCB designer must consider the ramifications of using either of the grounding methods. In general, the single ground plane eliminates any possible ground loops and provides for the lowest impedance path for the ground return.
Q: Won't noisy digital signals interfere with the analog inputs using a single ground plane?
A:This is a multi-faceted topic. Yes, a single ground plane can indeed create noise problems unless you are very careful about your total layout. Almost all of the return current will want to flow under the trace where it originated. So, there should be analog only portions of the board, and digital only portions of the board. Signals from one portion of the board should never cross over to the opposite portion of the board. In other words, route very carefully. If using an autorouter, make sure that you have specific rules that only allow routing within each designated portion. Always check the completed routing to verify signal integrity.
Q: So if the single plane is so good, why use a split at all?
A:In years gone by, high power devices were common with large currents running around the board. Ground and power splits were used to isolate one noisy section from another. In some cases it also separated high voltages from lower voltages. Lower power devices are now common place, so highly radiated current noise is not the issue it was at one time. If you plan early to use a single ground plane in your circuit and layout design, you will achieve success. However, power supply connections, clock speeds, board interconnect positions, heat sources and many other factors are outside the PCB designer's control. In these cases a split-plane may be beneficial. In this way the split can guide the return current in the right direction so that one noise source from one section of the board (like a switching power supply) does not interfere with another section (like the analog inputs.)
Q: Where do I begin?
A:You should always start your layout with the ground as your priority. One way to approach the layout is to utilize the split-plane concept. Create a digital portion and an analog portion to your PCB. Place a split between them so as to create a digital ground and a separate analog ground. Place the data converter over the top of the split. Place all your analog components in the analog portion, and the digital components on the digital portion. Only route signals for the analog portion within the analog ground area. The same is true for the digital, so keep all digital traces within the digital ground area. Once you have verified that all signals are routed appropriately, connect the two grounds together under the data converter. If you desire to have the single plane area, remove the split entirely.
Q: My PCB is single layer, what do I do?
A: This is challenging and your overall performance is not likely to come close to the datasheet performance. However, many have succeeded in making this work for their system. Not everyone needs full performance of a device, so less than ideal layouts can be implemented successfully. In this case, very careful steps must be undertaken for the complete layout. Sometimes good use of connecting wire on the non-copper side of the board is useful. The overall concept is to create a low impedance path for the ground. When laying out the board, try different component placements to try and get the best possible ground areas. Try to create some form of large, low inductance ground area, especially around the data converter.
PCB 板面布局的常见问题
• 接地技术
常见问题：如果转换器只有 16 位，我还用担心面板布局问题吗？
答：好的电路设计可能会因为板面布局不当而毁于一旦。即便只有 12 位系统，布局问题也是至关重要的。显然，转换器的分辨率越高，板面布局的问题就越重要。问题之一就是数字与模拟信号相混合交叉，导致噪声加大。还有一个问题就是接地处理欠妥的情况下，接地线迹会出现噪声问题，或返回电流被迫进入电路板上噪声较大的区域。
常见问题：我该在何处连接模拟与数字接地？
答：大多数数据转换器都要求模拟 (AGND) 与数字 (DGND) 接地之间不超过 0.3V，这通常会在产品说明书的最大绝对参数值部分加以明确。为了有效满足这一要求，数据转换器的两个接地之间必须存在低阻抗路径。
这样处理最有效的方法就是使用单接地层，将 AGND 和 DGND 直接连接到该层，而且尽可能靠近转换器的接地引脚。如果使用分离接地层，则应在转换器下使用尽可能大的铜接头将每个层的接地连起来，从而降低整体阻抗。
应考虑是使用接地层还是接地线迹，而且在可能的情况下，要将单接地层和分离接地层进行对比。
下列提供了一些数据转换器接地范例。
常见问题：我到底需不需要使用接地层呢？
答：最好使用接地层，因为能实现返回电流路径的最低阻抗。
问：只要连接了所有接地，就可以高枕无忧了吗？
答：从原理图的角度看，所有接地都连接到符号，也就是一个参考点。原理图仿真可在特定节点放上接地符号。通常该节点为 0V。事实可能与此大相径庭。如果您仔细分析已完成的双层 PCB，我们看到边缘侧有两个铜层被某种形式的电介质材料（通常为 FR4）分开。这是 PCB 上的一种电容。任何线迹的材料特性都会阻碍电子流动（电阻），而且也会有一定的电感值。此外，对于 PCB 上的任何孔或通孔而言也是这样。原理图和 PCB 的不同之处在于，任意两个接地点之间都存在实际的阻抗值。
问：若使用厚线迹的话，是否足够好？
答：或许很好，但通常对于高分辨率的模数转换器 (ADC) 而言不见得足够好。这主要是由于噪声使然。噪声可能是返回电流路径不佳造成的，也可能是来自外部来源的接地线迹所致。一些外部噪声源的产生可能是受 EMI/RFI 的影响或 AC 电力线影响的结果。接地线迹的工作通常像天线，会接收到杂散辐射噪声（如来自手机的噪声）。线迹电感也可能构成实际威胁，会在 ESD 等较短事件中损坏数据转换器。
问：我的 PCB 是双层的，而且我的接地层没有足够的地方。这会出现什么问题？
答：就 ADC 而言，噪声将会影响性能。我们会看到转换结果之间的代码差异远远大于预期。24 位转换器受噪声影响很容易损失一半的分辨率。如果受到噪声影响，应认真分析整体的板面布局。想办法让电路板的双侧都有尽可能多的接地区域。
常见问题：单接地层和分离接地层哪个更好？
答：这个问题很难回答，因为对此存在很多不同的观点。每个 PCB 设计人员都必须考虑这两种接地方法分别会产生什么样的影响。通常说来，单接地层会消除任何可能的接地环路，而且能为接地返回提供最低阻抗路径。
问：较大的数字信号噪声会不会干扰使用单接地层的模拟输入？
答：这是一个多方面的问题。是的，除非我们极为注意整体布局，否则单接地层确实会出现噪声问题。设计人员希望几乎所有的返回电流都在线迹源头流动。电路板上应该既存在纯模拟的部分也存在纯数字部分。来自电路板上某个部分的信号不应穿越另一部分。换言之，走线必须非常小心。如果使用自动布线器，则要确保制定具体规则，以便仅在每个指定的部分进行布线。此外还要确保完整布线以验证信号的完整性。
问：既然单层这么好，干嘛还要使用分离层呢？
答：多年来，高功率器件通常都在电路板上具有较高的电流穿过。接地和电源的分离可用于两个噪声部分相互隔离。此外，在某些情况下，分离可将高电压与低电压相隔离。较低功率的器件目前已比较普遍，因此极高的放射电流噪声问题不像过去那么严重了。如果较早就制定了在电路中使用单接地层的计划，并进行了相关板面布局设计，那么应该能够获得成功。不过，电源连接、时钟速度、电路板的互连位置、热源等众多其他因素则不在 PCB 设计人员的控制范围之内。在这些情况下，分离层可能有用。分离能够指导返回电流的正确方向，这样电路板上一个部分的噪声源（如开关电源）就不会干扰到另一部分（如模拟输入）。
问：我该从何处开始？
答：起点始终都应该是接地布局，这是需要优先解决的问题。开展布局工作的一种方案是利用分离层理念，即在 PCB 上分别创建数字部分和模拟部分，二者的分离能形成数字接地和独立的模拟接地。将数据转换器置于分离上。将所有的模拟组件都放在模拟部分，数字组件放在数字部分。模拟部分的路由信号都在模拟接地区域进行，同样，所有数字线迹都在数字接地区域之内。在确认了所有信号的适当路由之后，在数据转换器下连接这两个接地。如果希望使用单层区域，则移除分离整个。
问：我的 PCB 是单层的，该如何操作？
答：这极具挑战性，整体性能可能难以达到产品说明书的性能水平。但是，很多人都成功实现了整个系统的工作。不是所有人都需要发挥器件的全部性能，所以不太理想的板面布局也能成功实施。在此情况下，必须认真处理整个布局。有时可在电路板的非铜侧适当进行线路连接。整体理念就是为接地创建低阻抗路径。在进行电路板的布局时应尝试采用不同的组件放置方法，从而获得最佳的接地区域。想办法创建某种较大的低电感接地区域，尤其在数据转换器周边更应如此。
以上是我翻译的版本，若有不妥之处，欢迎各位设计师多多指正 ：）
对于精密或者低噪声设计，不管是单板还是系统级设计，有一个词记得时刻出现在脑海：回路。
当回路控制的思想(包括信号回路和噪声回路)应用于电子设计，很多问题分析和解决将变得容易许多。
个人观点