Stats

  • Locked Locked
  • Replies 10
  • Subscribers 64
  • Views 24371
  • 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

saving operating points

Charanraj Mohan

Hi,

I am writing something like this below,

'save M0,M1:all'

in the file saveop.scs and loading this in the model libraries setting of the ADE and getting the dc operating points in the simulation.

It worked well in AMS 0.35um, UMC 130nm, but not in ST 130nm :-(

Do you have an alternate way to this easier like above or to tackle this ??

I am using IC 6.1.6 130 version.


Thanks in advance.

Parents

  • It wouldn't be save M0.subcircuit_name:gm so that doesn't surprise me that it doesn't work.

    In spectre netlists, you always have this form:

    instName (conn1 conn2 ... connN) componentName param1=val1 param2=val2 ...

    The componentName can be a model, a primitive device, a subckt, a verilog-a model and so on - it doesn't matter. It's different from SPICE where the first character of the instance name says what kind of thing it is you instantiate. This makes it very easy to create more complex models by using a subckt.

    So, the model name that you're specifying on the transistor corresponds to the subckt name in the model file. What you are specifying in the save statement is the hierarchical instance name of the device you want to get the info save for. So for example, if your subckt model looked like this:

    subckt emos25 (d g s b)
    parameters w=1u l=2u
    MN1 (dint g sint b) ench w=w l=l
    R1 (dint d) resistor r=0.2
    R2 (sint s) resistor r=0.2
    ends emos25

    Then in your netlist you have:

    M0 (a inp 0 0) emos25 w=1u l=0.1u

    then you'd need:

    save M0.MN1:gm

    You need to know what the instance name is within the subckt that you are interested in.

    Regards,

    Andrew.

Reply

  • It wouldn't be save M0.subcircuit_name:gm so that doesn't surprise me that it doesn't work.

    In spectre netlists, you always have this form:

    instName (conn1 conn2 ... connN) componentName param1=val1 param2=val2 ...

    The componentName can be a model, a primitive device, a subckt, a verilog-a model and so on - it doesn't matter. It's different from SPICE where the first character of the instance name says what kind of thing it is you instantiate. This makes it very easy to create more complex models by using a subckt.

    So, the model name that you're specifying on the transistor corresponds to the subckt name in the model file. What you are specifying in the save statement is the hierarchical instance name of the device you want to get the info save for. So for example, if your subckt model looked like this:

    subckt emos25 (d g s b)
    parameters w=1u l=2u
    MN1 (dint g sint b) ench w=w l=l
    R1 (dint d) resistor r=0.2
    R2 (sint s) resistor r=0.2
    ends emos25

    Then in your netlist you have:

    M0 (a inp 0 0) emos25 w=1u l=0.1u

    then you'd need:

    save M0.MN1:gm

    You need to know what the instance name is within the subckt that you are interested in.

    Regards,

    Andrew.

Children
No Data

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.