Author Topic: 2 stage OpAmp  (Read 1711 times)

0 Members and 1 Guest are viewing this topic.

Offline kingkingsTopic starter

  • Newbie
  • Posts: 6
  • Country: eg
2 stage OpAmp
« on: May 24, 2020, 10:42:32 pm »
 

hello guys , i have been designing 2 stage Op Amp with this specs

and this is what i have done so far

 



my input voltage here is 1 V , i know i should decrease it because my supply is 3V , but to what value so i can saturate my mosfets and get the 75dB
« Last Edit: May 24, 2020, 10:44:06 pm by kingkings »
 

Offline Wimberleytech

  • Super Contributor
  • ***
  • Posts: 1134
  • Country: us
Re: 2 stage OpAmp
« Reply #1 on: May 25, 2020, 01:45:24 am »
Is it stable?
What is the phase margin?
Did it meet you SR spec?
You are burning a lot of current in the input stage...why?

Your gain depends on gm and r0, where r0 depends on channel-length-modulation...determined by your model.  Where are you getting your model?  Level 1,2,3, ?? 
Looks like a Cadence schematic...would be nice if you simulated it in LTSpice and provided an asc file.

As a starting point the ratio of Pm0/Pm1 should be twice Nm4/Nm0:  Pm0/Pm1= 2*2/6 = 4/6 NE 6/10...but close I guess.
« Last Edit: May 25, 2020, 01:57:09 am by Wimberleytech »
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2766
  • Country: ca
Re: 2 stage OpAmp
« Reply #2 on: May 25, 2020, 02:29:51 am »
Hi Wimberlytech and the group,

I have modelled lots of circuits in LTspice, but never tried IC design. I know that this can be done, I have heard that Linear Tech used LTspice for many of their IC designs.

I followed instruction that I found here:

http://www.blog-tm.de/?p=291

And inserted the PTM from here:

http://ptm.asu.edu/modelcard/2006/65nm_bulk.pm

I assume that this is the NMOS and PMOS models for 65nm process.

I used the W parameter to vary the geometry between the MOSFETs and built a 1:12 current mirror:



This gives M2 drain current is 1.2mA  (not the desired result)


Do I have set other parameters?



I assume that you need a PTM for the process that you are using?

The LTspice License agreement includes:

4. Restrictions. Licensee shall not ...

Snip ..

 This program is specifically not licensed for use by semiconductor manufacturers in the design, promotion, demonstration, development, or sale of their products. Specific permission must be obtained from Analog Devices for the use of LTspice for these applications.


I guess it is okay for educational use.

Regards,
Jay_Diddy_B

* Current Mirror.asc (5.91 kB - downloaded 48 times.)
« Last Edit: May 25, 2020, 02:53:50 am by Jay_Diddy_B »
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2766
  • Country: ca
Re: 2 stage OpAmp
« Reply #3 on: May 25, 2020, 03:01:59 am »
Hi,

There are other process models here:

http://ptm.asu.edu/latest.html

If I switch my LTspice model to use the 90nm BSIM3 I get a bunch of warnings but I get M2 Drain current 124uA which is better.

Model attached below.

Regards,

Jay_Diddy_B
* Current Mirror 90nm.asc (8.71 kB - downloaded 47 times.)
 

Offline Wimberleytech

  • Super Contributor
  • ***
  • Posts: 1134
  • Country: us
Re: 2 stage OpAmp
« Reply #4 on: May 25, 2020, 12:26:51 pm »
Hi Wimberlytech and the group,

I have modelled lots of circuits in LTspice, but never tried IC design. I know that this can be done, I have heard that Linear Tech used LTspice for many of their IC designs.

I followed instruction that I found here:

http://www.blog-tm.de/?p=291

And inserted the PTM from here:

http://ptm.asu.edu/modelcard/2006/65nm_bulk.pm

I assume that this is the NMOS and PMOS models for 65nm process.

I used the W parameter to vary the geometry between the MOSFETs and built a 1:12 current mirror:

(Attachment Link)

This gives M2 drain current is 1.2mA  (not the desired result)


Do I have set other parameters?


Regards,
Jay_Diddy_B

I have never used Level 54 model.  However, if this is a 65nm process, your voltages are too high.  I ran some curve tracer simulations using the model and it is clear that you need to keep voltages below about 1.2 volts.  But, there is still gate current...I question the model, frankly

You are not setting you channel length.  Not sure what LTSpice defaults to.  You need to set W=xx L=xx
« Last Edit: May 25, 2020, 12:31:12 pm by Wimberleytech »
 

Offline TheUnnamedNewbie

  • Super Contributor
  • ***
  • Posts: 1211
  • Country: 00
  • mmwave RFIC/antenna designer
Re: 2 stage OpAmp
« Reply #5 on: May 25, 2020, 12:30:27 pm »
Hi Wimberlytech and the group,

I have modelled lots of circuits in LTspice, but never tried IC design. I know that this can be done, I have heard that Linear Tech used LTspice for many of their IC designs.

I followed instruction that I found here:

http://www.blog-tm.de/?p=291

And inserted the PTM from here:

http://ptm.asu.edu/modelcard/2006/65nm_bulk.pm

I assume that this is the NMOS and PMOS models for 65nm process.

I used the W parameter to vary the geometry between the MOSFETs and built a 1:12 current mirror:

(Attachment Link)

This gives M2 drain current is 1.2mA  (not the desired result)


Do I have set other parameters?


Regards,
Jay_Diddy_B

I have never used Level 54 model.  However, if this is a 65nm process, your voltages are too high.  I ran some curve tracer simulations using the model and it is clear that you need to keep voltages below about 1.2 volts.

I ran your circuit with 1.2 volts and the results (current ratio) was pretty close.
You are not setting you channel length.  Not sure what LTSpice defaults to.  You need to set W=xx L=xx

I'm not familiar with predictive 65nm, but I suspect the 'D33' part in the transistor names of the original poster's screen shot refer to them being models for 3.3V IO transistors.

Jay_Diddy_B is indeed using the wrong transistors that will break past 1.2 V probably.

EDIT: I'm not even sure that the OP is using a predictive PDK. If this is an actual technology, it is very possible they can't even simulate outside of Cadence since those models are often encrypted and tied to Spectre.
« Last Edit: May 25, 2020, 12:32:50 pm by TheUnnamedNewbie »
The best part about magic is when it stops being magic and becomes science instead

"There was no road, but the people walked on it, and the road came to be, and the people followed it, for the road took the path of least resistance"
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2766
  • Country: ca
Re: 2 stage OpAmp
« Reply #6 on: May 25, 2020, 12:55:37 pm »
Hi,

I understand about the 1.2V limitation of the 65nm process.

I was looking at the original posters specifications:



So they need to do something 'special' like using 3V3 output transistors to build this op-amp in the 65nm process?

(I have done at lot with LTspice put not at the silicon level).

But the general idea of having a process model and then specifying different transistors with W=xx and L=yy is correct?

The default value for W and L  is 20u in LTspice.

Regards,
Jay_Diddy_B
 

Offline Wimberleytech

  • Super Contributor
  • ***
  • Posts: 1134
  • Country: us
Re: 2 stage OpAmp
« Reply #7 on: May 25, 2020, 01:25:18 pm »
Hi,


But the general idea of having a process model and then specifying different transistors with W=xx and L=yy is correct?


Yes

See example here:
 

Online SiliconWizard

  • Super Contributor
  • ***
  • Posts: 15800
  • Country: fr
Re: 2 stage OpAmp
« Reply #8 on: May 25, 2020, 02:14:01 pm »
The LTspice License agreement includes:

4. Restrictions. Licensee shall not ...

Snip ..

 This program is specifically not licensed for use by semiconductor manufacturers in the design, promotion, demonstration, development, or sale of their products. Specific permission must be obtained from Analog Devices for the use of LTspice for these applications.


I guess it is okay for educational use.

Slightly off-topic, but just to elaborate: AD excludes "semiconductor manufacturers". So that's not just OK for educational use IMO. As I read it, if you're not a semiconductor manufacturer (as per your main activity) but are just working at some company designing an ASIC for internal uses, that should be OK too. Take this with a pinch of salt, I'm no lawyer, but just designing some IC doesn't imply you're a "semiconductor manufacturer" IMHO.

Anyway, the OP could also learn how to use ngspice. It's fine for this kind of simulations, it's open-source, and the transistors models are quite good.

Although not for a 65nm process, but a 180nm one, I'm attaching a small ngspice lib I have used in the past, in case that could interest anyone.
« Last Edit: May 25, 2020, 02:18:49 pm by SiliconWizard »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf