Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Why will at low temperature Corner point Analysis( in cadence Virtuoso) fails?

Ali263

Junior Member level 3
Joined
Aug 21, 2020
Messages
29
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
229
I am doing corner point analysis of my design for all process corners and at different temperature.
However one amplifier fails at low temperature set? What can be the reason and how can it be fixed? In attach files, one can see the close loop, internal 2 stage OTA and its close loop gain. For corners at -10 temperture it fails.

How can i fix it?
 

Attachments

Last edited:

arthorios

Junior Member level 1
Joined
Jun 8, 2020
Messages
16
Helped
6
Reputation
12
Reaction score
5
Trophy points
3
Activity points
326
Show schematics, testbench and conditions for the simulation. Then, maybe, someone can have some insight.
 

Ali263

Junior Member level 3
Joined
Aug 21, 2020
Messages
29
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
229
is
Show schematics, testbench and conditions for the simulation. Then, maybe, someone can have some insight.
is it ok now? I have attached snaps
 

sutapanaki

Advanced Member level 4
Joined
Nov 2, 2001
Messages
1,222
Helped
484
Reputation
966
Reaction score
436
Trophy points
1,363
Location
US
Activity points
10,106
Why don't you check the operating point of your transistors in that specific failing corner?
 

arthorios

Junior Member level 1
Joined
Jun 8, 2020
Messages
16
Helped
6
Reputation
12
Reaction score
5
Trophy points
3
Activity points
326
Not enough, but close. So I will only guess.

You are using only one CMFB to set and sense the output CM level while controlling the 1st stage current sources. This is okay, but the problem you might have is that you leave the 1st stage output CM level dependent on the inversion level of the output stage transistor (PMOS here). So it might happen that the output CM of the 1st stage need to be too high/low to set the required VDD/2 at the output.

I would check what is the vgs-vth of the PMOS output transistors under failed corner. If this is too large, then give it more margin. Do simple DC op sims to debug this.
 

Ali263

Junior Member level 3
Joined
Aug 21, 2020
Messages
29
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
229
Why don't you check the operating point of your transistors in that specific failing corner?
I have a big chain and i check entire chain for 36 corners but only this amplifier fails for negative temperature.
can you explain how should i check OP when it is connected in closed loop .
 

sutapanaki

Advanced Member level 4
Joined
Nov 2, 2001
Messages
1,222
Helped
484
Reputation
966
Reaction score
436
Trophy points
1,363
Location
US
Activity points
10,106
Checking the OP in closed loop is not an issue. It is actually easier than doing it for the open loop case. It doesn't look you have a switched-capacitor circuit, so just enable DC analysis in cadence and print or annotate the operating point on the schematic. Do one simulation only for the corner that gives you trouble.
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,140
Helped
2,091
Reputation
4,186
Reaction score
1,938
Trophy points
1,393
Location
USA
Activity points
57,287
It looks like bias is simple so not the common
"my PTAT won't start up" problem.

There is always the possibility that some
corner or other is garbage from the foundry
modeling group. I've fought this a lot when I
was "inside foundry" and forced to run MC
analyses - would get runs where some
device(s) can be shown to fail WAT limits,
and the CAD weasels care not one bit.

The only way forward was to document
all of the fails-WAT MC iterations (which
were thankfully -not- random, but
pseudorandom repeatable from the same
seed any time you like), and disposition
any fails from those while running enough
extra iterations to mollify the Methodology
Harpies.

I would suggest that you lash up a fake
"WAT key" schematic imposing the major
WAT tests and ones that might matter to
an op amp (like FET Rout, which is seldom
measured other than as Vgs=0 leakage),
and see what "breaks out" for transistor
attributes at your failing iteration(s).

Now if it all goes out at low temp, processing
aside, that's probably something more basic.
Like maybe your VT has risen enough that
you have no headroom and thus no gain.

Scatter-plotting failing circuit attribute vs
the device characteristics you pulled from
that "WAT key" simulation (because of course
you followed my advice) might point you at
a highly-correlated suspect, and you could
decide whether normal processing or only
unrealistic parameter perturbations can
cause the failure.
 

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top