Stats

  • Locked Locked
  • Replies 5
  • Subscribers 126
  • Views 17929
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Spectre simulation of calibre extracted layout

moralope

 Hi,

I am trying to make a calibre extraction of the R+C+CC parasitics and I am getting some strange results. The layout is DRC and LVS clean and when I extract the layout without parasitics, my simulations work well. When I extract C+CC it also works well, but then when I include the R parasitics, the simulation starts to behave strange. 

To try to simplify and detect the problem, I only extracted one of the 2 nodes that are generating problems. The circuit contains 2 "pseudoresistor" connected in series, that is, 2 PMOS transistors with the BULK and SOURCE shorted. I have extracted the R parasitics (no cap) in the middle node.What is strange is that when I extract the R parasitics without any kind of parasitic reduction, the simulation of the cicuits does not work. But when I perform some reduction by combining several series resistor, the simulation works well.

I do not understand what is going on. It seems the problem is from Spectre, because the netlists for both cases seem correct to me. Please see the relevan extract of my netlist:

Without reduction:

     MM25 (MM25_d VhpP net020 net020) pch l=2e-07 w=3.5e-07 m=1 nf=1 \
        sd=620.0n ad=2.114e-13 as=2.198e-13 pd=1.88e-06 ps=1.92e-06 \
        nrd=1.72571 nrs=1.79429 sa=5.2e-07 sb=1.06e-06 sca=6.58985 \
        scb=0.00296926 scc=1.34332e-05

     MM29 (OUT VhpP MM29_s MM29_b) pch l=2e-07 w=3.5e-07 m=1 nf=1 sd=620.0n \
        ad=2.114e-13 as=2.198e-13 pd=1.88e-06 ps=1.92e-06 nrd=1.72571 \
        nrs=1.79429 sa=5.2e-07 sb=1.06e-06 sca=6.58985 scb=0.00296926 \
        scc=1.34332e-05

    rnet028_11 (net028_2 net028_7) resistor r=0.0206471
    rnet028_10 (net028_2 net028_10) resistor r=0.0431024
    rnet028_9 (net028_3 net028_7) resistor r=0.112412
    rnet028_8 (net028_3 net028_5) resistor r=10
    rnet028_7 (net028_5 MM29_s) resistor r=6.08436
    rnet028_6 (net028_5 net028_16) resistor r=4.24952
    rnet028_5 (net028_7 MM29_b) resistor r=11
    rnet028_4 (MM29_b net028_16) resistor r=4.2219
    rnet028_3 (net028_10 net028_11) resistor r=0.798652
    rnet028_2 (net028_11 net028_13) resistor r=0.0345872
    rnet028_1 (net028_13 net028) resistor r=10
    rnet028_0 (MM25_d net028) resistor r=6.09418
 

With reduction:

    MM25 (MM25_d VhpP net020 net020) pch l=2e-07 w=3.5e-07 m=1 nf=1 \
        sd=620.0n ad=2.114e-13 as=2.198e-13 pd=1.88e-06 ps=1.92e-06 \
        nrd=1.72571 nrs=1.79429 sa=5.2e-07 sb=1.06e-06 sca=6.58985 \
        scb=0.00296926 scc=1.34332e-05
    MM29 (OUT VhpP MM29_s MM29_b) pch l=2e-07 w=3.5e-07 m=1 nf=1 sd=620.0n \
        ad=2.114e-13 as=2.198e-13 pd=1.88e-06 ps=1.92e-06 nrd=1.72571 \
        nrs=1.79429 sa=5.2e-07 sb=1.06e-06 sca=6.58985 scb=0.00296926 \
        scc=1.34332e-05

    rnet028_5 (MM25_d net028) resistor r=0.01
    rnet028_4 (net028_5 net028_7) resistor r=10.1124
    rnet028_3 (net028_5 MM29_s) resistor r=6.08436
    rnet028_2 (net028_5 MM29_b) resistor r=8.47143
    rnet028_1 (net028_7 net028) resistor r=16.9912
    rnet028_0 (net028_7 MM29_b) resistor r=11
 

For me the 2 circuits should simulate in the same way because the only difference is the combination of resistors in series. But how to make sure that it is a problem of my circuit or a problem of spectre?

Have someone seen something like that before?

Thanks and best regards,

 moralope

  • It's fairly unlikely to be spectre, but one possibility might be that your circuit has multiple stable operating points - and it may be rolling into one or other depending on a slight change in starting conditions. I've seen that often as a root cause of such unexpected behaviour.

    The best thing would be to provide the entire data to customer support so that an AE can take a look.

    Regards,

    Andrew.

  •  Hi Andrew,

    I have checked for multiple operating points and I have not detected any problem. The circuit only have one operating point, but it is wrong after the extraction.

    However, my circuit is sensitive to leakage current in the 2 transistors. As these transistor are implementing a very big resistor in the order of the TOhm, then any small current flowing through the transistors can cause a large voltage drop. I have put gmin=0 to have a more accurate simulation. 

    When I increase the gmin to 1e-12 (default value), my simulation works again. So, my simulation works either for a "big" gmin or for bigger parasitic resistors (obtained after combining several small resistors).

    So, my questions are: Is the leakage current of the transistors not well modeled in the schematic? How does the leakage current change with the parasitic resistors? Is there a gmax value specified somewhere that depends on the gmin?

    Thanks.

    moralope

  • Hi, It seems I am the same calibre extraction issue with the parasitic R. Would you kindly tell me if you know the solution to this problem now ? thank you. Linfei

  • Hi Linfei,

    I was not able to solve this issue and it is still a mistery for me. I asked many experts around and they were also surprised with that.

    I am still interested to solve this problem because I am facing it again, so if you have any news please let me know.

    Best regards,

    moralope.

  • Hi, I know my problem now. it is what Andrew suggested. my circuit had several operating point. My suggestion is that you run DC analysis first to see if both schematic and post-layout simulation results match. if not, you can compare the netllist to find out the difference. sometimes, the schematic instance does not cover everything, at least that's the cause in my case. hope it helps. Regards, Linfei

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.