ERROR (OSSGLD-18): and not able to run simulation

Dear cADEUser,

Would you please post the contents of your stimulus file(s)?

1. I'm wondering if you told spectre the syntax was spectre syntax. This is done by a line at the beginning of the file "simulator lang=spectre". 

2. However, there may also be a syntax issue with the use of brackets in an include file and I think if you provide the contents of the files, it will provide the information needed to provide a more accurate response.

Shawn

Content of this file is what I have pasted in my earlier thread. It's just these two lines

_vpd_data_enb (pu_data_enb 0) vsource wave=[0 0 1n 0 1.015n vcchbm 3n vcchbm] dc=0 type=pwl
_vpu_data_enb (pd_data_enb 0) vsource dc=pu_enb type=dc

Dear cADEUser,

cADEUser said:

Content of this file is what I have pasted in my earlier thread. It's just these two lines

Thank you! It is evident you did not include the prefix required to identify the syntax as spectre syntax. Did you try including the line "simulator lang=spectre" as the first line of the file? 

Shawn

"simulator lang=spectre"
_vpd_data_enb (pu_data_enb 0) vsource wave=[0 0 1n 0 1.015n vcchbm 3n vcchbm] dc=0 type=pwl
_vpu_data_enb (pd_data_enb 0) vsource dc=pu_enb type=dc

I still get the same ERROR. Does the above look correct ?

BTW : I have used many stimulus without any problem in the past. I never had to use the line  "simulator lang=spectre". 

Dear cADEUser,

cADEUser said:

still get the same ERROR. Does the above look correct ?

There are no quotation marks around the first line. Please just make the first line:

simulator lang=spectre

Shawn

Hi Shawn, 

Thanks a lot for your help. If I add the simulator lang=spectre and run spectre standalone from Unix prompt then it is working. So by adding "simulator lang=spectre" works but I have to run the spectre using the binary directly.  From ADE Gui, I can't past the nestling even with this line added : simulator lang=spectre. It keeps failing with the ERROR :  ERROR (OSSGLD-18): The command character after '[' in the NLP expression '[0 0 1n 0 1.015n vcchbm 3n vcchbm] dc=0 type=pwl

Dear cADEUser,

cADEUser said:

f I add the simulator lang=spectre and run spectre standalone from Unix prompt then it is working.

Well, that is good news! Thank you for letting us know!

cADEUser said:

rom ADE Gui, I can't past the nestling even with this line added : simulator lang=spectre. It keeps failing with the ERROR

I was not sure, when I first saw your post, but you may need to escape your brackets. In essence, try changing your file to the following:

_vpd_data_enb (pu_data_enb 0) vsource wave=\[0 0 1n 0 1.015n vcchbm 3n vcchbm\] dc=0 type=pwl
_vpu_data_enb (pd_data_enb 0) vsource dc=pu_enb type=dc

Shawn

Dear cADEUser,

cADEUser said:

f I add the simulator lang=spectre and run spectre standalone from Unix prompt then it is working.

Well, that is good news! Thank you for letting us know!

cADEUser said:

rom ADE Gui, I can't past the nestling even with this line added : simulator lang=spectre. It keeps failing with the ERROR

I was not sure, when I first saw your post, but you may need to escape your brackets. In essence, try changing your file to the following:

_vpd_data_enb (pu_data_enb 0) vsource wave=\[0 0 1n 0 1.015n vcchbm 3n vcchbm\] dc=0 type=pwl
_vpu_data_enb (pd_data_enb 0) vsource dc=pu_enb type=dc

Shawn

Aha....thanks Shawn. Yep...that's the trick. After adding \ to escape the brackets, it is working. Many thanks for your help.

A little explanation as to why the escape is needed.

Stimulus files are a very long-standing feature in ADE and were mostly useful from the days when many of the netlisters were flat netlisters and translated schematic names into numeric net names in a flattened hierarchy. If you wanted external stimulus from a text file, you ideally wanted a way to reference a name that appeared on the schematic without having to worry about what it got translated to in the flat netlist - i.e. what number - and instance references (e.g. for current-controlled sources) also needed to be translated. So the idea is that you can use the [] "NLP" syntax in the file to reference a schematic name, e.g.

[#netname]  - for example [#/I1/net2]
[$instname]  - for example [$/I3/V3]

Then ADE (or rather the underlying netlisting system) takes the stimulus file, and translates it into the actual net names/instance names used in the netlist, and then that file is included in the resulting simulation netlist. You'll see that your stimulus file is not directly included in the spectre netlist - it includes a copy of the file which has been copied into the netlist directory, and this copy has had any translations applied.

The stimulus file can still be useful even in the days of hierarchical netlisters, because it takes care of any mappings performed on illegal characters or reserved words that have been used in the schematic names (by illegal or reserved, I mean for the simulator). However, that's not very common (other than bus syntax, for example) and it's often just as easy to escape any characters that you know will be translated.

If you really don't need this translation, it's simpler to reference your stimulus via the Setup->Model Libraries or the Definition Files field of the Setup->Simulation Files form, both of which simply add an "include" into the spectre netlist referencing your file, and hence don't need the escaping of the vector syntax  you've used. This is mentioned in this article ADE gives ERROR OSSGLD-18 on including stimulus file from Simulation File Setup on support.cadence.com which shows up if you search for OSSGLD-18, the error code you got.

Hope that helps clear things up!

Andrew.

Thanks a lot Andrew of the details explanation. It's really helpful. Much appreciated for the details.