手机音频layout走线规则谁能总结一下

LZWsimba

最近开始做手机音频设计，对layout走线规则及PCB检查不清楚。
请高手指点一二，提供资料更好。
给个方向也可以。

LZWsimba

5＃大虾能否提供相关的资料，谢谢！

LZWsimba

我手头只有高通的英文资料但只是简介，恳请有这方面经验的大虾指点。

zhubelly

有谁有吗？

octhey

做个标记，以便查阅！

alee_love

音频信号，避免和高速线平行；避免靠近电源线和射频线；两侧均包地，地线宽度要大于20mil；音频线的上下层均为地层。

zhubelly

也想学一下。

yiweidianzi

1.Run the differential (signal+, signal-) pair TOGETHER all the way from the MSM codec to the audio amplifier driver.
2. Run the differential pair such that the distance (separation) between them is constant at every point along the way (keep them TOGETHER and as close as possible).
3. Run the differential pair identical (match trace width/length/thickness and impedance).
4. Run the differential pair with GROUND GUARD FIELDS from the rest of the board (ground needs to be of lowest potential and, if possible, run on ground planes).
5. Run the differential on the quiet side of the PCB. Dedicate one side of PCB to have all analog signals.
6.Run the differential pair with the minimum distance from MSM codec to the PMIC speaker amplifier inputs.
7.Keep the input filter stage close to the PMIC speaker amplifier inputs.
8.Avoid running the differential signal traces from one layer to another, because transversing through vias could bottleneck your signal and cause a voltage drop. If you do run the signals from one layer to the next layer, make sure the vias can handle the current. Run the pair on the same board plane as much as possible.
9.Avoid separating the differential pair, because it could loose its immunity against common mode noise.
10. Run the pair AWAY from any digital signals (clocks, digital grounds, other high speed
switches).
11. IPC-D-275 states that for an internal conductor a minimum of 4 mil (0.004 inches) of
conductor spacing is needed for voltages between conductors of 0-15 V DC or AC peaks.
12. Minimize MSM codec to transducer signal trace length (keep the system to close proximity).
13. Avoid sharp turns of signal traces.
14. Avoid running signals close to RF/antenna, especially the input signals.
15. Place Cin close to PMIC speaker amplifier.
16. Single-ended input configuration trace from MSM codec to PMIC needs ground fills
[br]<p align=right><font color=red>+5 RD币</font></p>

yiweidianzi

1，敏感走线（Mic，receiver，speaker等差分线）远离干扰源（如天线，battery走线，高速数字走线，开关电源）。
2，敏感走线尽量用GND包起来；条件允许，可以将个别干扰源也屏蔽起来。
3，Mic，Receiver，Speaker等差分信号线，需要严格差分走线（与线路匹配的相同的宽度，长度，厚度和阻抗），尽量避免差分对之间的分开——这样可以降低抑制共模噪声的能力。建议0.2mm。
4，尽量将敏感电路放在屏蔽罩内。
5，在敏感线路上预留滤波电路（磁珠、电容）。
6，Receiver走线上不宜并太大电容，过大的负载电容会导致放大器自激。
7，音频电路的接地要特别注意：
■ 基带音频IC需要充分接地（多打地孔到参考地）。
■ 不要和表层地连接。
■ 最好直接打孔到主参考地。
8，第一级放大器要靠近声源，尤其是Mic，滤波电路要尽可能的靠近Mic；
10.Mic信号是最敏感的，最好布在中间层，尽量少跨层走；
11.耳机HPH_R和HPH_L彼此分开走线，彼此平行走线会增强共模噪声；
12.在receiver、耳机线路上靠近音频功放输出端增加“磁珠”，抑制天线辐射对音频电路的干扰。
13.ESD器件就近布局，EDA设计时，走线应先进入ESD器件，再进入需要防护的器件；
14. Mic的ESD器件（TVS管）不能放在天线的净空区域。[br]<p align=right><font color=red>+5 RD币</font></p>

xxz840

有没有这方面的文档？

a910903

thanks~~~~

aman7890

1：The analog audio tracks are very sensitive to noise .Therefore all vias & traces must be guarded by gnd.
2: the differential signals include EPP/EPN , LSP/LSN, MICP1/MICN1(MIC1) and MICP2/MICN2(MIC2). These signals should be routed in a differential manner to minimize noise coupling effect.
3: MIC1/MIC2 trace width is 0.1mm minimum.
4: EPP/EPN trace width is 0.2mm minimum(if possible 0.3mm) whereas for LSP/LSN should be 0.3mm due to output of amplifier and also to reduce impedance.
5: HSL/HSR are single-ended line. Trace width is 0.2mm minimum(if possible 0.3mm)
6: For MIC supply lines (VMIC and VUMIC), a 330pF capacitor should be placed near to BB chip, the corresponding capacitor ground should be connected to clean ground. This is needed to stabilize the MIC supply.
7: MICP1/MICN1, MICP2/MICN2, EPP/EPN, LSP/LSN & HSR/HSL lines routed on Layer5 guarded by GND planes on Layer4 & Layer6.

FrankTsang

thanks~~~~

joneyoung

谢谢！学习

echo_057

非常好，学习了~[em01]

373353088

支持支持支持支持

liangqitou

thanks
[em01]

jang2lin

<B>以下是引用<i>yiweidianzi</i>在2011-10-8 13:27:33的发言：</B>

1，敏感走线（Mic，receiver，speaker等差分线）远离干扰源（如天线，battery走线，高速数字走线，开关电源）。
2，敏感走线尽量用GND包起来；条件允许，可以将个别干扰源也屏蔽起来。
3，Mic，Receiver，Speaker等差分信号线，需要严格差分走线（与线路匹配的相同的宽度，长度，厚度和阻抗），尽量避免差分对之间的分开——这样可以降低抑制共模噪声的能力。建议0.2mm。
4，尽量将敏感电路放在屏蔽罩内。
5，在敏感线路上预留滤波电路（磁珠、电容）。
6，Receiver走线上不宜并太大电容，过大的负载电容会导致放大器自激。
7，音频电路的接地要特别注意：
■ 基带音频IC需要充分接地（多打地孔到参考地）。
■ 不要和表层地连接。
■ 最好直接打孔到主参考地。
8，第一级放大器要靠近声源，尤其是Mic，滤波电路要尽可能的靠近Mic；
10.Mic信号是最敏感的，最好布在中间层，尽量少跨层走；
11.耳机HPH_R和HPH_L彼此分开走线，彼此平行走线会增强共模噪声；
12.在receiver、耳机线路上靠近音频功放输出端增加“磁珠”，抑制天线辐射对音频电路的干扰。
13.ESD器件就近布局，EDA设计时，走线应先进入ESD器件，再进入需要防护的器件；
14. Mic的ESD器件（TVS管）不能放在天线的净空区域。
+5 RD币</p>

学习了。。。留个脚印

rpg_9527

学习了1

YFB0823

学习了，谢谢分享！