Nanosim Simulation: Can't locate resistor model

[nanavaras6284]

Hi,

I am a student working on digital IC design. I have completed the layout of the design and need to estimate the power consumption using Nanosim from the netlist generated from the layout using Calibre PEX.

When I run the nanosim simulation on the spice netlist, it returns an error.

Error:Nanosim:0x30201054:File "./netlist.sp", line 783, column 0, format SPICE: Can't locate resistor model

I have added the following line to the spice netlist generated by Calibre PEX.

.lib "tech.lib" tm

tech.lib file includes all the model files of resistors, capacitors and MOSFETs.
'tm' refers to the typical mean model files. Nanosim does read these SPICE commands and includes the model files, but I am still getting the same error message.

Please guide me, on how to check where I am going wrong.

 

[se3]

hi, I also have the same problem. if you have found the solution, would you share here?

 

[nanavaras6284]

I havn't figured this one out.

This only happens with the netlist generated by Calibre PEX.
When I tried with Spectre or hspiceD netlist generated from Cadence Analog Environment, this error does not occur.

I also tried to copy the netlist header from hspiceD netlist to the Calibre PEX netlist but it didn't help. Still shows the same error.

Sorry.

 

[se3]

hi,
I actually still cannot solve too, but now i can run a netlist generated using calibre PEX by someone else. it has to be set up as a model. a guideline has been posted here:
https://www.cadence.com/Community/b...a-subcircuit-netlist-with-spectre-in-ade.aspx

if you find it confusing (like I did), just reply this message with your problem.

sigit

 

[nanavaras6284]

Hi Sigit,

Isn't the link provided for simulation with Cadence's Spectre. Did this work with Nanosim?

regards,
Saravanan

 

[se3]

nanosim works with hspice/ spice netlist files, right?

1) if you have the layout and the schematic as well as the RCX/ PEX extractor like assura and calibre, then the work will be very simple; you just extract your layout, and then by using config for hspiceD you can set up a post simulation with hspiceD simulator.
to get the hspice netlist, after you set your config file for hspiceD, just click the botton to generate the netlist in ADE, and save the neltlist as a *.sp file. later you run this file using nanosim.

2) if you only have a hspice post-sim netlist (as in my case), then you can either setup your simulation setting using your hspice/ spice knowledge to make netlist for the power supply, control voltage, input signal and so on; or , like in my case, you can first make a cadence model for that post-sim netlist (this is the purpose of the link i gave you), and then put all required voltage/ signal sources, then generate the hspice netlist, and then use the netlist in nanosim.

 

[nanavaras6284]

My case is the first one. But the problem persists.
I will look into this.

Thanks for your replies.

 

[ankitgarg0312]

Error:Nanosim:0x30201054:File "./netlist.sp", line 783, column 0, format SPICE: Can't locate resistor model

open file "netlist.sp" and go to line 783 ..
copy paste that line in forum...
i may be able to answer your problem....

 

[nanavaras6284]

Thanks.

The lines 781, 782 and 783 are copied below.

rX7/X17/R2 N_AUDIO_IN[7]_X7/X17/R2_pos N_X7/X17/9_X7/X17/R2_neg RDIFFP3 w=3e-06
+ l=9.6e-06 $SUB=N_VDD!_X3/X12/R2_sub
dX7/X17/D3 N_GND!_X3/X12/M7_b N_X7/X17/9_X7/X17/D3_neg ND AREA=7.5 PJ=10.2284

I am assuming that the error it shows is in the resistor model RDIFFP3 (lines 781 and 782). But Nanosim does not show any error while compiling the models.

regards,
saravanan

 

[ankitgarg0312]

i feels that this is your design resistor and not parasitic.

i also expect that you will be having a resistor model with name "RDIFFP3" in your models.

do a trick:
your line 781 starts from rX7/X17/R2 as of now , make it XrX7/X17/R2
"add a X in front of that line" and try to run it.

if this clears your this error i can give you reason for this problem else there is one more possibilty
first try above then we will see further

 

[nanavaras6284]

Yes. Now the error does not occur on that line after adding the Prefix "X" to it.

Why does this happen? How can I solve this problem?

regards,
saravanan

 

[ankitgarg0312]

your model card has resistor in form of subckt def
.subckt RFIFFP3 ....
grep this resitor name in model file , you will find it
now to instantiate subckt you have to start with X as that first letter of device name.
your prelayout netlist will have X in front

this problem occurs because of extraction.
i can't comment on this part.
check with mentor calibre extraction person or forums , they will find out reason why it start with R and not X.
there may be some switch required to help you there

 

[nanavaras6284]

Yes the model file shows RDIFFP3 as subcircuit.

Thanks a lot. I will try to fix this.