基础的二级运算放大器管子尺寸设计问题

luoweihua

刚学CMOS不久，现在需要做仿真，没什么经验，想问一下大家看到电路是怎么分析管子W/L宽长比的，我在网上看到的资料层次不齐，求指导！谢谢大家！

transistor7

去参考学习一下gm over ID的设计方法
http://web02.gonzaga.edu/faculty ... /documents/gmid.pdf

https://designers-guide.org/foru ... _ID_Methodology.pdf

http://aice.sjtu.edu.cn/msda/dat ... D_Sizing_Method.pdf

https://people.eecs.berkeley.edu/~boser/presentations/2011-12%20OTA%20gm%20Id.pdf

https://analog.intgckts.com/gmid-design-methodology/

xuwenwei

网上看个什么硕士论文啥的 基本的原理应该都能清楚了吧 或者看看那几本圣经
我也刚学，一般W/L是通过电流 和 gm确定的，电流是功耗决定 gm是增益确定 而且你还得选取合适的Vdsat，当然里面还有很多东西 比如如果你有miller补偿 的话 你的负载电容确定的话 gm会先计算出来，w/L定下来后 L的值就是看工艺啊 或者mismatch 之类的 再去定义了，这里面东西还是挺多的，是需要去看书的

luoweihua

transistor7 发表于 2020-5-8 08:44
去参考学习一下gm over ID的设计方法
http://web02.gonzaga.edu/faculty/talarico/EE406/documents/gmid.pd ...

行，看见很多资料都有这个GM/ID，但是并不知道是啥，谢谢！

luoweihua

transistor7 发表于 2020-5-8 08:44
去参考学习一下gm over ID的设计方法
http://web02.gonzaga.edu/faculty/talarico/EE406/documents/gmid.pd ...

请问有没有网址或者文件分享，我这直接打开不了线上PDF文件，或者是说有什么操作可以在线上也能看PDF

transistor7

luoweihua 发表于 2020-5-8 23:14
请问有没有网址或者文件分享，我这直接打开不了线上PDF文件，或者是说有什么操作可以在线上也能看PDF

...

Traditionally operating a MOS transistor in strong inversion region is the analog designers choice in their design space[1, 2]. Transconductance of a MOS transistor is . We have three degrees of freedom.

EKV Model is a physical model, was proposed by Enz, Krummenacher, and Vittoz from EPFL.

The channel current in weak inversion region is given by

(1)

where,
and
n is subthreshold slope factor (~ 1.5 in 180nm CMOS tech).

Trans-conductance in weak inversion region is

(2)

(3)

gm/id methodology is used to size transistors, particularly in short channel devices or deep sub-micron technologies.
The following data is generated over a reasonable range of and channel lengths
Generate data for the following over a reasonable range of gm/ID and channel lengths

• Transit frequency (fT)
• Intrinsic gain (gm/gds)
• Current density (ID/W)
  

These parameters are (to first order) independent of transistor width, which enables “normalized design”.

In a MOS transistor as increases, generation efficiency decreases. is maximum in weak inversion, and almost constant over a large range in this region.

2011-12 OTA gm Id.pdf (898.41 KB, 下载次数: 159 )

2020-5-9 03:17 上传

点击文件名下载附件

Gm_BY_ID_Methodology.pdf (958.22 KB, 下载次数: 99 )

2020-5-9 03:17 上传

点击文件名下载附件

gmid1.pdf (1.01 MB, 下载次数: 88 )

2020-5-9 03:17 上传

点击文件名下载附件

Lect08_gm_ID_Sizing_Method.pdf (1.47 MB, 下载次数: 88 )

2020-5-9 03:18 上传

点击文件名下载附件

transistor7

luoweihua 发表于 2020-5-8 23:14
请问有没有网址或者文件分享，我这直接打开不了线上PDF文件，或者是说有什么操作可以在线上也能看PDF

...

Finding out gm for hand calculations at a given operating point
Perform simple dc and transient analysis of a schematic comprising of a transistor of required W/L and applied Vds and Vgs. Now there are two ways to find out gm of the transistor at the specified operating point.
1. In Analog Design Environment (ADE) click Tools > Result Browser. In the browser window select do-to-dc and select for transistor from the list and see its gm from the list of given parameters.
2. In ADE click Results > Direct plot > Transient operating point. Now screen goes to the schematic. click on the transistor. window opens. scroll to see gm. gm/id is also mentioned as gmoverid. Various model parameters can also be seen by selecting Model Parameters from Dirent plot and select any device.

Plotting gm and gm/Id
Use the same circuit designed above with a transistor and suitable bias voltages.
By default spectre doesnt save the operating point of the devices to keep the psf file slim. however we can force spectre to save all the operating points. Follow the below steps to do this.

1. Make sure spectre is being used as the simulator.

2. create oppoint.scs from our favourite editor and save it in your cadence work directly. make sure you have write permission to this directory. In the oppoint.scs file write this

save N0ppoint

here N0 is the instance name of the NMOS transistor used in the schematic. We can find out more about command save from spectre user guide.

3. now click ADE -> options -> select waveform tools : AWD

4. now sweep Vgs of the transistor and hit netlist and run in ADE

5. go to the result browser as: ADE > tools > result browser, then, schematic->psf/ -> Run 1 -> DC to DC -> N0, this gives the DC operating points saved.

6. Right click Gm and get the gm plot

7. Add this file as a model library file just like what you usually do to setup Spectre. Make sure the path to oppoint.scs is correct. It is important to note that AWD was used as the waveform tool instead of wavescan.

8. Go to ADE and click menu session, then save script. A window will pop up and that is the first OCEAN script you are going to use. Please note that this ocean script file will be saved in your default cadence directory. From the script file, you can find out that all these setups you made
for simulation in here. OcnWaveformTool set the wave viewer to AWD. Command Simulator selects Spectre as the simulation engineer, so on and so forth.

You have to add few lines to this simple script file to save the DC operating point parameters you are interested in (copy this text exactly):

selectResult(‘dc)
plot(getData(“N0:gm”))

ocnPrint(?output “~/gmid.dat” ?numberNotation ‘scientific
getData(“N0:gm”),getData(“N0:id”),getData(“N0:vdsat”),getData(“N0:cgs”))

Here, ?output means all data will be saved to a file called gmid.dat. You can modify the tag line “~/gmid.dat” in order to have the gmid.dat file saved any directory of your choice; otherwise the gmid.dat file will be saved in your root directory. getData selects the parameter you want to save.

9. Now you can load this file and run the simulation again from CIW window by typing:

load(“gmid.ocn”)

10. Go to the root directory (or where ever you saved the file) and you can find “gmid.dat”. All the parameters you want, gm, Cgs, Id, Vdsat (Defined as vd) are saved here.

11. Plot the required curves using any scientific program like MATLAB.

魔陈公仔

好好看看这个文档，能学到很多。

luoweihua

魔陈公仔 发表于 2020-5-9 17:20
好好看看这个文档，能学到很多。

好的，谢谢！！！！！！

hjc19951212

魔陈公仔 发表于 2020-5-9 17:20
好好看看这个文档，能学到很多。

这种资料从哪里搞到的呀