psf format different when simulation is run from ADE or in command line

Laurent,

This is because in the top one you are using the results browser for the entire set of simulations (you might only be running one, but ADE could allow multiple runs because of sweeps or corners). In other words, you're looking at the psf/testName/psf dir rather than (e.g. 1/testName/psf dir - the number being one of the points). If you go over one of the output cells in the ADE results and do Right Mouse->Results Browser it would open the specific point only and then you should see what you are seeing in the bottom ViVA.

Hope that makes sense.

Andrew

Thanks Andrew.
While you were answering, I realized my mistake and misunderstanding.

ExporerRun0/psf/testName/psf : the nets are saved as waves
ExporerRun0/1/testName/psf : the nets are saved as scalars

And of course when I RMB->Open Terminal and launch runSimulation, I re-create this ExporerRun0/1/testName/psf (i.e, scalar).

Now my questions are: 
How is the ExporerRun0/psf/testName/psf created?
Is it possible (with a spectre argument or option) to make the ExporerRun0/1/testName/psf contain waves rather than scalar?

It's not really that the nets are saved as waves for psf/testName/psf. What happens is that for the psf/testName/psf dir, ADE creates a runObjFile which collates the individual point results together as a family, and hence when opening that you get waveforms instead (because there might be more than one point simulated and even with a single point it's a waveform of one point).

You'd have to surround the analyses statements in spectre with some kind of sweep to achieve the same thing:

tempSweep sweep param=temp values=[27] {
  dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
  dcOpInfo info what=oppoint where=rawfile
}

This is a sweep of one point. I'm not sure why you would want to do this though?

Andrew

It's not really that the nets are saved as waves for psf/testName/psf. What happens is that for the psf/testName/psf dir, ADE creates a runObjFile which collates the individual point results together as a family, and hence when opening that you get waveforms instead (because there might be more than one point simulated and even with a single point it's a waveform of one point).

You'd have to surround the analyses statements in spectre with some kind of sweep to achieve the same thing:

tempSweep sweep param=temp values=[27] {
  dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
  dcOpInfo info what=oppoint where=rawfile
}

This is a sweep of one point. I'm not sure why you would want to do this though?

Andrew

ok, clear. I understand now the utility of this runObjFile.

Why do I want a psf with waves?
I save ADE outputs (ocean expressions) and would like to apply them, thanks to an ocean script, to a psf created by a spectre unix command.
example : 
This ADE expression : 
is saved in an ocean script as : offset=(abs (difference (VDC "/VOUT") (VDC "/VREF")))
If this this ocean expression is applied on a psf created from spectre unix command (i.e, containing scalar if the DC analysis has no sweep), it returns the following error : 
*Error* difference: can't handle (nil - nil)

That expression should work if VDC() returns a scalar (it certainly can do that) It's just subtracting two scalar values and then taking the absolute value - that should be OK. The issues is that VDC() is returning nil. That's because the argument to the VDC has been given as a schematic  name rather than a netlist name (it begins with a "/" and could use "/" as the hierarchy separator). For this to work, it needs the runObjFile in the point psf directory to point to the netlist directory, where it uses the mapping data to map from schematic names to netlist names.

If you change the expression to (abs (difference (VDC "VOUT") (VDC "VREF"))) then it would work fine (the leading slash is removed).

Andrew

ok. Thanks for the explanation. I really thought that VDC() returned nil because it's a scalar in psf and not a wave.
So I need to adapt the ADE output expressions to support netlist names.

Laurent.

kkdesbois said:

So I need to adapt the ADE output expressions to support netlist names.

By the way, Is there a function to transform the ADE output expressions written as schematic name to expression written as netlist name?

Not really. The trouble is that the mapping could be complex if the name happened to use a spectre reserved word, but in general you could use:

asiMapNetName("/the/path/to/maestro/results/maestro/Interactive.10/2/TRAN_ONLY/psf" list("/diffOut"))

(it copes with the "psf" dir or the one above - the "data" dir).

That's just for the net name part - it doesn't transform the entire expression.

Andrew