DAC靓声要诀—TDA1541 NOS DAC布线技术帖译文

小鬼头

一、前言

Layout即排板布线，是DAC制作中一个非常重要的环节。用我下面译文的原作者K.Y.Wang的话来说，DAC的声音至少一半来自Layout。换言之，DAC要靓声，必须要有好的Layout作支撑。

有经验的DIY友都深知模拟放大线路中地线排布的重要性，DIY坛上也经常出现网友为排除模拟地线引入交流声而求助的帖子。相对于模拟放大线路，DAC由于高速数字电路所引发的排板布线要求远远要高。如果直接套用模拟线路的技术、经验去处理高速数字电路的排板布线，则必定中招无疑。

我小鬼头在若干年前，曾对一台VCD机DAC芯片附近的地线进行修改，不但没有取得以往在模拟线路上的收效，反而令DAC芯片迅速发热烧掉...55555。自那时候起，我就很留意这方面的技术，但可惜的是，国内各类公共电子书刊对DAC的DIY介绍少之又少，谈及DAC Layout技术的更是凤毛麟角。。。。。及至我上网后，才通过互联网找到这方面的信息（下面的英文帖是使我受益的一个重要帖子），并买到这方面的技术书籍，明白了“低频模拟线路中信号是走电阻最小的路径，高速数字电路中信号是走电感最小的路径”等等道理，大大开了眼界。

半年前，我运用所学知识，在TDA1541 NOS DAC上首次尝试用铜皮进行Layout的改进，取得了良好的效果，DAC的音场表现力等方面明显提升。前段时间，我参与了论坛TDA1543四块并联、运放作I/V和LPF的NOS DAC的数字部分PCB布线意见，简单试听下，该DAC的高频表现已然胜出我手头上的马兰士CD72。及后再改为电阻作I/V、运放作LPF的四块并联TDA1543 NOS DAC试验板，经我们坛上一位富有DIY经验的海外网友试验，反馈回来的消息是：普通优质元件装制的此试验板，比他下足功夫摩改的的原TDA1543 DAC要靓声。。。。。

本帖内容主要译自DIYAUDIO论坛上DIY高手Kuei Yang Wang与法国学生网友的对话，。Kuei Yang Wang又名Thorsten Loesch，一名神秘高手，音响DIY的理论、知识和见闻高深莫测，用台湾一个个人网页的说法是“他的DIY知识深度和广度令你吃惊”。他对音箱、胆机、数码音响这几方面尤其擅长，TNT网站上有他的TDA1541 NOS DAC等DIY文章，也曾见一个网页上他仿制Wilson喇叭的专文。。。。半年前我所说TDA1541的+5V电源常被菲利浦故意做为+6V，就是他在此帖中透露的。。。。老外的大师、专家、高手不厌其烦地指导他人。。。真令人感概。

因时间关系和本人水平的十分所限，我只将我去年看帖时记在笔记本的9页记录基本照抄出来（稍有整理），有些英文没能译出，文字方面也很粗糙，错误和不便之处在所难免，请谅。

此外，若对高速数字电路Layout技术的，我还再次推荐国内难得一见的好书——H. Johnson的《高速数字设计》以及Mark I.Montrose著 《电磁兼容和印刷电路板理论、设计和布线》。看了这两本书，相信你会大大加深对有关Layout技术的了解。。。。第二本据说有姐妹篇，而且更实用，好象已在国内出版。。。谁能提供此书的信息？

http://www.dearbook.com.cn/book/viewbook.aspx?pno=TS006664



http://www.erji.net/read.php?tid=97705&fpage=&toread=&page=2

小鬼头




  
级别: 骑士
发帖: 169
威望: 230
金钱: 447
注册时间:2004-03-01
      
--------------------------------------------------------------------------------


个人认为走线布局引发的信号完整性（SI）等问题在DAC的Layout非常重要，有人称DAC的声音至少一半来自Layout...有关这方面的知识，建议看看这本H Johnson所著的经典著作《高速数字设计》：

http://www.china-pub.com/computers/common/info.asp?id=19367

DAC靓声要诀—TDA1541 NOS DAC布线技术帖译文

　本书是信号完整性领域的一部经典著作，英文版已经重印了将近20次。全书结合了数字和模拟电路理论，对高速数字电路系统设计中的信号完整性和EMC方面的问题进行了深入浅出的讨论和研究。其中不仅包括了关于高速数字设计中EMC方面的许多实用信息，而且包括了许多有价值的测试技术。另外，书中详细讨论了涉及信号完整性方面的传输线、时钟偏移和抖动、端接、过孔等问题。 本书通俗易懂，是高速数字设计人员必备的参考书，实用性很强，独特地将理论与实践方法相结合，适合从事模拟和数字电路设计的相关人员使用。本书可以作为大专院校相关专业师生的教学参考，对于体系结构设计人员、EMC专家、印刷电路板设计和布线专业人士也是一本极具价值的参考书。


电磁兼容和印刷电路板理论、设计和布线

DAC靓声要诀—TDA1541 NOS DAC布线技术帖译文

内容简介：
  本书从理论、设计和布线的角度分析研究了电磁兼容（EMC）和印刷电路板（PCB）所涉及的问题，全书内容共有9章。第1-3章介绍了EMC的基本原理、PCB中的EMC以及元件设计中的EMC，第4章论述了PCB中镜像面的原理与特性，第5章和第6章详尽在阐述了PCB中的旁路与去耦以及传输线的设计原理。第7-9章就信号的完整性与串扰、PCB走线终端以及PCB布线中的接地原理进行了论述。
    本书集理论和实践于一体，适合于那些涉及逻辑设计和PCB布局设计的

吻子

谢谢鬼版提供资料[em05]

tmdqqs

音乐虫子

HQ

aeon

4059

小鬼头

感觉国内的DIY技术水平。。。。这是基本的东西。。不说了。你明白的。;)

万健

什么时候出新的1543，1541DAC啊？

4059

小鬼头

第32帖：

Kuei Yang Wang []
diyAudio Member

Offline
Registered: Nov 2002
Location: City of the Sanjian


  Post #32  
Konnichiwa,
quote:
Originally posted by Bricolo
If the DAC has 3 separate supplies. They go on the board, pass though the regs, and arrive at the DAC supply pins.
But how to control the ground return path?


By using seperate traces (suitably arranged with trace width and fill to give low inductance of course and closely coupled to our groundplane in our 4-layer PCB) for the return.

The loop:

PSU +V
Reg +in
Reg +Out
IC +V pin
IC -V pin (often mislabeled gnd as it doubels as signal ground)
Reg -V pin (often mislabeled gnd as it doubels as signal ground)
PSU -V

Can be closed without even ONCE refering or connecting to the circuit "ground". That way our imaginary electrons in the current flow go exactly where we want them to.
quote:
Originally posted by Bricolo
Do you mean connecting the analog (digital) supply's ground close to the DAC's analog (digital) ground pin, on the copper plate?

This way, all the supplies's grounds will be connected together at the copper plate. Right?


Yes. basically, "signal ground" and "ower Supply Return" are separated out into the respective loops and thus controlled.
quote:
Originally posted by Bricolo
The copper plate will be connected to the ground of the other components somewhere on the board?

Why would it? All components relevant to a given current loop blong conneted to the relevant returns for that current loop and nowhere else.
quote:
Originally posted by Bricolo
Or will they have separate wires going to the player's star ground point?  

What is "star ground"? A methode to maximise loop area and length and thus problems.

Sayonara


    [回应：如果有一台DAC有3个独立电源，他们在板上，通过稳压过去，然后到达DAC的引脚。这怎样控制地返回路径？]
    通过使用独立分离的走线作为返回（适合于按排宽的走线，当然，地铺成低电感，并且就近耦合到地平面，这是我们的4层PCB）
    环路是：
    PSU +V （正电源）
    REG +in （正稳压输入）
    IC +V引脚
    IC -V引脚（通常被标错为GND，因为它作为信号地被双重使用）
    REG -Vin（通常被标错为GND，因为它作为信号地被双重使用）
    PSU -V（负电源）
    即便是没有参考电路的“地”，这个环路是能够闭合。
    这样，我们想像电流是按我们所想地流动。

    [回应：你是指将模拟/数字部分电源的地靠近于DAC的模拟/数字的地引脚，在铜平面上吗？这样，所有电源的地都将一起连到铜平面上，对吗？]
    是的。基本上，“信号地”和“电源返回”被独立分离在各自的环路，并回此得到控制。

    [回应：铜平面将连接到板上某一处元件的地吗？]
    为什么这样？与电流环路有关的所有元件都连到他的电流环路相关的返回，其它地方都不是。

    [回应：或者他们有分离的接线连到CD机的星形地？]
    “星形地”是什么？这是令环路面积、长度最大的一种方法，因此有许多问题。

第36帖：

There are three fundamental axioms in this:

1) Ground isn't
2) Consider where the current(s) flows
3) Make sure current(s) flows where you want it and via the shortest possible, lowest impedance loop


    。。。。
    这里有三个基本的公理：
    1、Ground isn't （“地”不是）
    2、考虑电流的流动
    3、确保电流按你所想的流动，并且尽可能走最短和最低阻抗的环路

第38帖：

Tthe -15V and the +6V (in most Philips applications this is 6V not 5V) are the analogue section and there is a corresponding PSU pin, the other PSU Pin and Ground are logic.


    大多数菲利浦机中的TDA1541的+5V是使用+6V电源。这个+5V和-15V是模拟部分，并有一个相关的电源引脚，其余电源脚是和地是数字的。

If you must share one dual polarity, common ground supply between DAC analogue, DAC digital and receiver using a groundplane with "scatter grounding" may be the lesser evil in context, leading to the best possible perfomance from a compromised design.

In that case carful mechanical arrangements (physical layout, orientation etc.) becomes of tantamount importance to avoid circulating PSU ground noise through the section of the groundplane where signal current flow. This often implies carefully introduced partial breaks in the groundplane, producin

小鬼头

第24帖：

Kuei Yang Wang []
diyAudio Member

Offline
Registered: Nov 2002
Location: City of the Sanjian


  Post #24  
Konnichiwa,
quote:
Originally posted by Bricolo

In fact, in my case, it's for a DAC without the reciever (it will be in the player itself, in IIS). Can I use the ground plane as a ground for the components, so?

I would prefer to avoid doing that.
quote:
Originally posted by Bricolo

If not, what are you calling current loops (effecting the signal)?

quote:
Originally posted by Bricolo

The ground of the regs,


Of course.
quote:
Originally posted by Bricolo

the decoupling caps,


Certainly
quote:
Originally posted by Bricolo

the I/V resistor?


Obviously.
quote:
Originally posted by Bricolo

If we shouldn't connect anything to the groundplane, for those making theyr PCB themselves, wouldn't be the easier solution to use a double side board, leave one totally with copper (this will be the groundplane), and the other side for the signal lines, plus a groundfill for the components ground?


That is not a bad option, except it makes for difficult ground routing. I prefer dead bug hardwiring with the IC's wrapped in Copperfoil and soldered to a copper sheet adhered to additional PCB Material for a number of perfectly good reasons, all relating to this kind of thing.

Really good PCB's for the 1541 (single) would likely be 3 or 4 Layer minimum, I dread the concept of parallel 1541's....
quote:
Originally posted by Bricolo

If I understood it correctly, you advice to do something like on the shielded cables: connect the shield to ground, but don't make any current flow in it (don't let it be a return path). Am I right?  

Pretty close.

The common (dumb) use of groundplanes seems similar to that of NFB, it can hide a multitude of sins and once designed with this "groundplane" you stand zero chance to ever "debug" the problems introduced in the circuit by doing so anyway, so hope the problems are going to be pretty small anyway, if not - no-one will notice anyway.

Sayonara

    [回应：我这里是用于DAC，没有接收部分，因为我的是整台CD机。我可以用地平面作为元件的一个地端吗？]
    我喜欢避免这样做。

    [回应：如果不可以利用地平面作为元件的地端，你称的影响信号的电流环是什么？是稳压、退耦电容、I/V电阻的地吗？]
    稳压的地当然是，退耦电容、I/V电阻也是。

    [回应：如果我不应把东西连到地平面，作为做PCB本身，使用双面板不容易解决问题，即让双面板一面作为地平面，另一面除了信号走线外全面铺为地，并且将元件围起来？]
    这是一个不差的选择，除了它会令走线困难之外。我喜欢dead bug硬接到用铜箔包裹的IC，并焊到粘附在PCB板材料上的铜片，为了一定数量的原因，所有都与这些东西相关。
    真正好的PCB给TDA1541用，最少将是3层或4层板，我害怕并联TDA1541这种做法。

    [回应：如果我正确理解，你是建议要做一些事情，比如在屏蔽电缆上：将屏蔽层接地，但不让任何电流流过他（不让返回电流流过它，不让它成为返回电流的路径）。对吗？]
    相当接近。
    地平面的共用是近似于NFB负反馈，他能掩盖了相当多的过失。一旦你用一个地平面作设计，你将得到零的机会去debug掉由电路带来的问题。

第26帖：


Kuei Yang Wang []
diyAudio Member

Offline
Registered: Nov 2002
Location: City of the Sanjian


  Post #26  
Konnichiwa,
quote:
Originally posted by Bricolo
Avoid what? Using the groundplane for the components, or placing the DAC in the player?


Groundplane for components.
quote:
Originally posted by Bricolo
So, everything on the board


Of course.
quote:
Originally posted by Bricolo
With your dead bug hardwiring, the IC is shielded with the copperfoil, and this is soldered to the copper sheet.
But what are the grounds of the components soldered to?
Only point to point, or also to the copper sheet?


Point to point, with seperate supplies for the different sections (so no shared ground returns) with the copper sheet/groundplane used STRICTLY to connect the two digital grounds on receiver and DAC and DAC digital to DAC analogue. The rest is insulated from the groundplane.
quote:
Originally posted by Bricolo
What do you c

小鬼头

二、译文


全部译自K.Y.Wang的发帖。原英文帖子为《 Parallel TDA1541A non-o/s DAC Kits 》（TDA1541A并联的NOS DAC套件）中K.Y.Wang与法国学生网友Bricolo的问与答，连接如下
http://www.diyaudio.com/forums/s ... 0043&highlight=

第12帖：

Kuei Yang Wang []
diyAudio Member

Offline
Registered: Nov 2002
Location: City of the Sanjian


Re: Parallel TDA1541A non-o/s DAC Kits  Post #12  
Konnichiwa,
quote:
Originally posted by siu sin man tho
I was prepare one set of the Parallel TDA1541A non-o/s DAC Kits.

Good luck. Good digital sound is to at least 50% in correct grounding and PSU decoupling and the TDA1541 is by far from ideal in layout, making the ground layout optimisation for ONE IC a nice challenge. Now doing for two is nothing I'd relish.
quote:
Originally posted by siu sin man tho
1. All caps was philips MKP caps.

Barely okay for decoupling. Look first and foremost at low inductance, secondly on the microphonics. Dielectric et al are modestly unimportant, as the "refresh rate" for these cap's is quite fast.
quote:
Originally posted by siu sin man tho

2. Sanyo OS-con
3. all 1% Dale metal film resisters.

Fine.
quote:
Originally posted by siu sin man tho

4. OFC 2mm thick PCB with Groud plate to low the noise.


Hmmm. Groundplane is good, AS LONG as you don't use it to close any current loops. If you use the groundplane to also the ground currents from IC's life get's interesting.
quote:
Originally posted by siu sin man tho

5. Digital & analog rectifier cap use Elna high performance series
Gold label caps (25V 3300uf).


More important is the rectifier and the snubering of the transformer parasitic resonance.
quote:
Originally posted by siu sin man tho

6. diode use MBR 160 or Schottky series to lower the noise.


Good. Use a "Zobel" across the secondary - R = aparent DCR (primary & secondary) of transformer, Cap as large value as feasible but not so large that significant current flows at 50Hz.
quote:
Originally posted by siu sin man tho

Three Analog Output Stage for user choose.


Best is direct coupled, filterless (but use Anti Sin(x)/(x) Filter), transformerless 7308 (Common Cathode stage per channel), biased directly from the -2mA offset of the DAC at a few 100mV, low anode voltage, choke or CCS load. Watch linearity though, this arrangement is a bit critical, the Valve operates near zero bias. But the short chain of: Chip -> Resistor -> Grid (cathode direct to ground) -> Cap from Anode to output works best from where I stand.

Sayonara


    好的数码音响的声音至少50%来自正确的接地和电源退耦，而TDA1541本身在布线使用时远非理想。给一块TDA1541做好接地已经是一项挑战。现在你做两块，我会relish。

    [回应：全部使用菲利浦的MKP电容]
    作为退耦很少是OK的。首先要看低阻抗，其次要看麦克风效应。介质已经不是很重要，因为这些电容的刷新速度已经很快。

    [回应：用SANYO的OS-CON电容，1%的DALE金属膜电阻]
    Fine(很好)。

    [回应：数字机模拟整流的电容使用ELNA高性能的金字电容3300UF/25V]
    更重要的是整流器和变压器寄生谐振的抑制。

    [回应：使用MBR160或肖特基二极管降低噪声]
    good.用一个Zobel(茹贝尔)网络接在变压器的次级，使用的电阻，其阻值接近于变压器的直流电阻，电容尽可能大，但不能明显让50HZ的交流电流流过。

    [回应三种模拟输出级让用家选择]
    最佳的是直耦，无滤波器（但使用反sin(x)/x滤波器），无变压器接法的7308胆放大（每一声道是共阴放大），由DAC的-2mA偏移电流得到的100mV来偏置，使用低的阴极电阻，使用电感或恒流源负载。留心线性，这里是有些严格，胆接近于零偏置工作。但短的路径是DAC芯片——至电阻——至栅极（阴极直接接地）——至阳极的输出电容，将在我的情况下工作得最佳。



第16帖：

Kuei Yang Wang []
diyAudio Member

Offline
Registered: Nov 2002
Location: City of the Sanjian


  Post #16  
Konnichiwa,
quote:
Originally posted by Bricolo
Thorsten, do you mean that the groundplane musn't be connected to any component? Only one connection to the ground  

Depends/not quiet. What I strongly recommend however is not to use the groundplane for closing current loops effecting

swuzzy

lm3886

返璞归真

AKMY5

外行的人会不以为然，然内行的听了头晕，做起来头痛！要求高的行家却会着迷。。。
有幸拜读鬼版大作！！！[em11]

小鬼头兄说的：
“用一个Zobel(茹贝尔)网络接在变压器的次级，使用的电阻，其阻值接近于变压器的直流电阻，电容尽可能大，但不能明显让50HZ的交流电流流过”
立马受精！[em11]下班马上就去试一下！！！



“低频模拟线路中信号是走电阻最小的路径，高速数字电路中信号是走电感最小的路径”等等道理”

上面这话总结得太精彩了！偶们正是这样做的，可是却由于缺乏理论指导，提炼不出这样精华的认识来！感谢鬼版！


但是，我隐约感到！关于Layout排板布线，除了地线的排布外，供电线路的排布和信号线的排布也是有得好好考究的！怎么样让各系统间各高速的数字和模拟IC间不相互干扰，地线的排布是第一重要外，供电的电源的屏蔽和排布算第二重要了！否则会相互间串扰，不能忽视！至于信号线，大家看看电脑主板就知道了，除了大量地进行“蛇形机动”以外，对于高频高速的信号通道，两面还有大面积地线“护送”。

希望能再拜读鬼版这方面的文章！

赤兔

[em11]

twoguitar

相信对于1541,这几款, 新的板本应该达到一个新的高度...

jpyj299

<>学习了，谢鬼版。</P>