Question on OCEAN standalone evaluation

When you refer to a signal name in one of the access functions (e.g. v(), i(), etc), then if the name starts with a "/" it is a name using the schematic namespace. If it doesn't begin with a slash, it is in the netlist namespace. In the schematic namespace, the names have / as the hierarchy delimiter, and will ultimately need to be mapped to whatever name was actually used in the netlist and then saved into the result database. In order to do this mapping, the ADE netlisters save some additional information in the map and amap directories in the netlist directory. This information is then consulted to do the same mapping when somebody wants to access a result signal using the output database. However, for that to work, the results access has to know where the map directories are. This can be done if the simulation is run from OCEAN or ADE, by virtue of a line in the runObjFile which tells it where the "netlistDir" is. In the absence of this, I think it assumes it is in ../netlist. However, if this mapping data is missing, it cannot do the mapping and hence cannot see signals using the source database namespace.

If you omit the slash, it's always using the netlist name and so that will work regardless of whether the mapping directories are present. However, you do need to then know how any name was mapped - this mapping can happen due to illegal characters, spectre keywords and so on that have been used.

In your specific example, outp on the schematic ended up as outp in the netlist, so it was relatively straightforward to resolve.

Regards,

Andrew. 

Hi Andrew,

Thanks for the reply.

My next questions then would be:

- Which is the "mapping directory"? I see two directories in the spectre/spectre/schematic/netlist directories - "map" and "amap". Which is the relevant one?

- What is the OCEAN command for specifying the location of the mapping directory?

Thanks in advance

As far as I know, it's the amap dir that's needed (this is consistent with experiments I tried). There's no public API to create the runObjFile (which would then allow arbitrary location of the netlist directory), but provided there is a netlist directory at the same level as the psf directory, and the netlist dir contains the amap, the mapping works fine even without the presence of the runObjFile (i.e. if the simulation has been run standalone outside of OCEAN) (the output below has been trimmed a bit):

unix_45> ls -R schematic
schematic:
netlist/  results.psf/

schematic/netlist:
amap/        

schematic/netlist/amap:
__multiplefiles_amap_format__  analogLib_npn_spectre.inst
__new_amap_format__            analogLib_pmos4_spectre.inst
__nmp_amap_format__            analogLib_pnp_spectre.inst
__simulator_information__      analogLib_res_spectre.inst
ampTest.inst                   analogLib_vdc_spectre.inst
ampTest.net                    analogLib_vsin_spectre.inst
ampTest.port                   supply.inst
amplifier.inst                 supply.net
amplifier.net                  top_level_map.inst
analogLib_cap_spectre.inst     top_level_map.net
analogLib_idc_spectre.inst     top_level_map.port
analogLib_nmos4_spectre.inst

schematic/results.psf:
ac.ac                 logFile                     tran.tran
dcOp.dc               modelParameter.info         tran.tran.0.sig.tmp
dcOp.sens.dc          outputParameter.info        tran.tran.dat
dcOpInfo.info         primitives.info.primitives  tran.tran.sig
designParamVals.info  sens.output                 tran.tran.sig.tmp@
element.info          spectre.out
finalTimeOP.info      subckts.info.subckts

Then I can do:

ocean> openResults("schematic/results.psf")
"schematic/results.psf"
ocean> selectResult('tran)
stdobj@0x14d09048
ocean> outputs()
("/net9" "/net12" "/out" "/V2/PLUS" "/vdd!"
    "/vin" "/vss!" "/I3/V0/PLUS" "/I3/V2/PLUS" "/I7/gnode"
    "/I7/net7" "/I7/net18" "/I7/net29" "/I7/net39"
)

If it can't find the mapping info, outputs() will names in the netlist namespace.

Regards,

Andrew.

 I could get it to work partially, but not fully. If I place the amap directory in the right place (under schematic/netlist), I can see that the output names are in the schematic space. However, the expressions still do not evaluate correctly. Is there any other command that needs to be issued before the expressions?

ls schematic/
AC1.psf/  netlist/

cd schematic/

 artil

> openResults( "test_simulation/schematic/AC1.psf" )
> selectResult('ac)
stdobj@0x145c3110
> outputs()
("/AOP" "/AOPIN" "/INM" "/INP" "/net017"
    "/net028" "/OUTM" "/OUTP" "/V3/PLUS" "/V_IMON1/PLUS" ...
> gain_1k = dB20(value((VF("/OUTP") - VF("/OUTM")) 1000))
*Error* difference: can't handle (nil - nil)
 

Oh, I think I figured it out.

 The psf directory name has to be "psf". It can't be anything else. In that case, things work fine.

Does it work if you use v("/OUTP") etc instead of VF()? If you've not done selectResult('ac) first you'd need to do v("/OUTP" ?result 'ac) .

The VF, VT functions etc were historically for ADE rather than OCEAN and certainly in IC5141 are quite dependent upon the simulation having run in ADE. We've improved that in later releases (I didn't check this specific issue) but thought I'd suggest you try v()

Regards,

Andrew

I checked, and this is only the case if you use the VF(), VT() type ADE functions (even in IC615). If you use the v() OCEAN function it works fine if the results directory is not called "psf".

Regards,

Andrew

Hi Andrew,

Unfortunately, I am facing the same problem.

WARNING (OCN-6054): The output '/a/b/c<node1>' you selected does not exist. Type outputs() to see the list...., etc. etc.

Things I did: 

1) I did check outputs() to make sure the name was correct

2) I checked runObjFile file and it does show: "netlistDir" "../netlist"

3) I plotted the signal fine and sent it to calculator to check the name -- it's still showing '/a/b/c<node1>'

However, taking some pointers from your post, I changed "/a/b/bus<n1>" to "a.b.bus<n1>" and that worked instead. But may be for this example it worked Ok b'cos of similar names. But technically, they are not the same ----

"/a/b/bus<n1>" -- bus is a net under subckt definition of instance b) while

"a.b.bus<n1>"  --- bus is a node of instance b, and it may or may not be connected to the net 'bus' as per b's subckt definition).

So I am worried I cannot generalize this solution. Looking forward to your help.

I'm not sure why you don't think they are the same thing.

A name with "/" at the beginning is the hierarchical name as it appears in the schematic. A name with "." as hierarchy delimiters (without a leading slash) is using netlist names - so it will be bus<n1> inside subckt instance b inside subckt instance a. That sounds the same to me.

Without seeing the details, it's hard to be certain why this didn't work - probably we'd need to see your data and understand the versions of the tools you're using - and for this, you may be better off going to customer support.

Regards,

Andrew.

I don;t have much clue what's going on here. In save outputs, if I give "allpub" its saving everything and I am plotting fine -- not sure in what format it is accepting the net names internally. However, if I select something selectively from schematic, netlist it, I see this in netlist:

save I0.rxcpdqrx.ctlep\<5\> ....

And spectre (while running) gives me a warning:

WARNING (SPECTRE-8281): `I0.rxcpdqrx.ctlep<5>' is not a node nor an instance name.

And if I change the netlist to this

save /I0/rxcpdqrx/ctlep\<5\> ....

Spectre crashes:

 ERROR (SFE-874): "input.mod.scs" 8028: Unexpected operator "/". Expected end of file or end of line

It seems like the hierarchical delimiter is "." for psf data but not for nelist. There is a clear disconnect. Things run fine for signal nets but croak for bus nets (probably because of "<" ">" special characters). By the way, initially, I had already tried special charcters in v("/a/b/c\<node1\>), but it gave me warnings:

PARSER WARNING at line 192 column 35 of file *ciwInPort*

*WARNING* (Parser): character found after backslash is not meaningful - /I0/rxcpdqrx/ctlep\<5\>