Stats

  • Replies 4
  • Subscribers 125
  • Views 1865
  • Members are here 0

Virtuoso ADE dc analysis incorrectly turned to multiple design point mode

SimbaG

Key Issue:

My Virtuoso ADE environment consistently treats simulations as multiple design point simulations, even when there is only one "design point."

Observed Behavior:

  1. Even when performing a very simple DC analysis:
    • All sweep options are disabled.
    • No corner simulations or parameter variations are included.
    • A completely new ADE Maestro view is created.
  2. The environment still incorrectly identifies the simulation as having multiple design points; while actually there is only one design points.
  3. This behavior seems abnormal, given the minimal configuration for such a simulation.

Impact on Functionality:

This issue also affects the plotting capabilities in the Main Form. Upon attempting to plot, the following error occurs:

ERROR (WIA-1006): Unable to plot expression <v("/Iin" ?result nil)>
because it does not evaluate to an object that can be plotted, like a waveform or
parametric wave. See the Visualization & Analysis Tool documentation for information
about the types of objects that can be plotted in Visualization & Analysis Tool. Only
the expressions that evaluate to those objects can be plotted.

Additionally:

  • The expression v("/Iin" ?result nil) does not work for plotting.
  • The expression v("/Iin" ?result dc) also fails to produce a plot.
  • However, the expression VDC("/Iin") works correctly and yields the expected results.

Environment Versions:

Here are the relevant version details of the tools I am using:

virtuoso -W
sub-version IC23.1-64b.43

spectre -W
sub-version 23.1.0.442.isr7

Thank you in advance for your help!

  • The Direct Plot form is designed to plot waveforms here, and it's getting confused by the lack of a sweep. The resulting expression is wrong - using ?result nil makes no sense. Similarly, since you only did a DC operating point, using ?result 'dc (it should have a single quote in front of the analysis name, or you could use "dc" too) won't work either because no DC sweep was performed. You can however use:

    v("/Iin" ?result 'dcOp)

    When VDC() is plotted or v("/Iin" ?result 'dcOp) as a graph, there has to be some x-axis - so in the absence of any variables, the design point is used. There is a design point - only a single design point though for a single simulation - I don't see anything in what you've said above that suggests there's multiple design points.

    So, other than the Direct Plot form not being better behaved with only a DC operating point, I don't see anything wrong here.

    Andrew

  • in reply to Andrew Beckett

    In a previous version of Virtuoso (likely IC6.1.8, in ADE L), I remember the following behavior:

    1. When performing only a DC sweep, the "signal type output" would be displayed as a single number.

    2. Even when requesting to plot a number or a single design point waveform, the result would appear as a text box in the waveform window (unfortunately, I don't have a screenshot of this).

    However, in the current version, this behavior seems to have changed:

    • Now, the signal type always appears as a waveform, and I cannot directly get a numerical output.
    • To achieve a number, I must manually write expressions like VDC("/signal").
    • The Results -> Plot Outputs -> DC, is always grey, even if I save the DC operation point in DC analysis.

    Is this change due to the introduction of ADE Explorer? If this is the expected behavior, I suppose I just need to adapt to it.

  • in reply to SimbaG

    This has been an option for a long time - maybe you've turned it on for some point. Use Results→Plotting/Printing Options and check the Scalar Outputs for Single-Point Simulations checkbox in the Graph Annotations section (I can't upload a screenshot at the moment as the forum software is being difficult).

    For your points above:

    SimbaG said:
    When performing only a DC sweep, the "signal type output" would be displayed as a single number.

    If it was a sweep, a single number wouldn't have been displayed (it wouldn't make sense). if it wasn't a sweep, a single value wasn't displayed as far as I know.

    SimbaG said:
    Even when requesting to plot a number or a single design point waveform, the result would appear as a text box in the waveform window (unfortunately, I don't have a screenshot of this).

    This is the option I mentioned above.

    The Results->Plot Outputs->DC is for DC sweeps, not DC operating points. Results→Print→DC Node Voltages would give you the scalar outputs. Or you have to use VDC() or v(... ?result 'dcOp) to do this. This has always been the case.

    Andrew

  • in reply to Andrew Beckett

    What I expected is when there is only one design point, Viva XL Waveform will plot it as "scalar outputs"
    As the following screenshots shows. Is it related tio EvalType in ADE? 

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.