Simulation files and bus syntax

If you're using the stimulus file field in ADE, it gets passed through a pre-processing option to allow you to use "schematic" names in the netlist, which can then have any mapping applied to them that happened during netlisting.

Because of this pre-processing, the \ you are entering is being stripped off (you'd have to use a double backslash). A better approach is to use the OSS mapping syntax. For example, if you do:

v1 ([#bus<0>] 0) vsource type=sine freq=1M ampl=1
v2 ([#bus<1>] 0) vsource type=sine freq=2M ampl=1.5
v3 ([#bus<2>] 0) vsource type=sine freq=3M ampl=2.0
v4 ([#bus<3>] [#/gnd!]) vsource type=sine freq=4M ampl=2.5

You should then end up in the netlist as:

v1 (bus\<0\> 0) vsource type=sine freq=1M ampl=1
v2 (bus\<1\> 0) vsource type=sine freq=2M ampl=1.5
v3 (bus\<2\> 0) vsource type=sine freq=3M ampl=2.0
v4 (bus\<3\> 0) vsource type=sine freq=4M ampl=2.5

or whatever those bus names got mapped to during netlist. Note that there's a problem in IC613/IC614 where this (by default) doesn't work properly with busses (the backslashes get missed out). It's OK in IC5141. The CCR is 752498 - and the workaround is to switch back to the mapping scheme used in IC5141 - enter envSetVal("asimenv" "mappingMode" 'string "oss")

We also have a CCR to get the above [#...] syntax documented more clearly (it is right now, but hidden away in the Open Simulation System manuals, rather than being in the ADE manuals).

Regards,

Andrew.

 Hi Andrew,

Thanks very much for this. Mixed results though. It will now parse the file. However in the input.scs file that it generates for the design from the schematic, bus nodes that were previously listed as e.g. bus\<1\> are now listed as bus_1. Then, if I select one of those from the schematic for being saved and plotted, this appears in the save statement as  bus\<1\>, with the effect that they are not recognised as nodes and not saved or plotted. Any ideas? (I'm not stuck though because I can use "nmp" mapping and double backslashes for now). 

One more related question: in my design I had a bus called BLin<1:36>. When I simulated this, node BLin<35> and only that one caused problems - it seemed to recognise that node as already existing, although it's nowhere else in my design. when I changed the name of the bus to e.g. BLInputs<1:36> the problem went away. Have I hit on a reserved word or something like that?

 Thanks

Sim Bamford

Hi, 

I am trying to include a stimulus file using an OCEAN script with IC 6.15/MMSIM 12.1.

It connects a voltage source to a net bus<1>.

The OSS syntax [#...] doesn't seem to work (Unexpected '[' or unexpected '#' error). Bus<1> doesn't work either (unexpected '<').

In the input.scs the net seems to be output as bus\<1\>.

Using bus\<1\> and bus\\\<1\\\> work (i.e. no errors at read-in) but in all cases the net comes up as floating and is removed.

Using the suggested option by Andrew with bus_1 in the stimulus file still leads in the net being removed. 

I am assuming I am missing some mapping happening at some point after the initial netlisting.

The net is not at the top level of the hierarchy but lower down.

Any ideas would be greatly appreciated.

 Thanks,

Kostas 

Kostas,

This ought to work - are you using envSetVal("asimenv" "mappingMode" 'string "oss") ?

If you've changed it, you probably would need to re-start ADE and also force a Netlist->Recreate.

If it doesn't work, please contact customer support - we need to investigate why.

Andrew.

Hi Andrew,

thanks for the reply.

Just for the record, simulating with ADE worked as expected in the end (even without the OSS mapping). It was a mistake on my side.

I didn't manage to get OCEAN to work consistently. I have given up on that approach a while ago.

Thanks anyway,

Kostas