Hi everyone,
I was simulating a simple RC circuit to find it's frequency response using the following two third party Murata capacitor models GRM155C71H104JE19 and GRM155C71H103JE19 in the following circuit.


I received the following error message: Multiple instances of "C1" as shown:


Please guide me how to solve this unexpected behaviour. The simulation is attached to this question.

Thank You,
With Regards,
Srinjay Bhattacharya

 

Hello,

I am not an user of ltspice, but both subcircuits use C1 in them.
Perhaps that causes the multiple instances of C1.

Bertus

 

hi sbya,
Stripping out the GRM...19 Cap and creating a *.net model I get this.??
Shows 3 terminals.?
Where did you get the net list.
E

 

hi sbya,
Stripping out the GRM...19 Cap and creating a *.net model I get this.??
Shows 3 terminals.?
Where did you get the net list.
E

Hi ericgibbs,

My bad, please ignore the extra "C" in the line : .MODEL SUBCKT GRM155C71H104JE19 C port1 port2 and rectify it by removing the extra "C" for this and for GRM155C71H103JE19 as well.
Still the same error message pops up.

Thank You,
With Regards,
Srinjay Bhattacharya

 

hi sbya,
Reducing to only one component still shows error!.
E
I have also downloaded the model from the web site.

 

See

 

h sbya,
Look at this simple demo.
E

 

hi Alex,
An explanation of what you did to make the simulation work , would be helpful.
E

 

hi sbya,
I have made two LTS models, using the nets.
E
I can post the nets if you wish, then you can make your own models.

Posted.!
E

 

See

Hi Bordodynov,
Thanks for correcting the simulation file. Please also mention the changes you made to make the simulation work.

Thank You,
With Regards,
Srinjay Bhattacharya

 

,model and .subckt are independent spice directives. It is not proper to combine them. .model works for devices known to the spice engine like diodes, transistors, and switches. The number of parameters that can be specified in known and fixed. .subckt is a different command with a different syntax an semantics. The list of parameters is unknown and not fixed a priori. It is used for opamps, comparators, and other complex devices. The behavior is described in terms of devices known to the spice engine.

To see what other changes were made, export the text from the schematic to a file and do a text compare on the files. The results should be readily apparent.

 

hi papa,
I did try without the MODEL text, got this error , ref image.

I cannot see any differences in the remainder of the text/s, as posted by the TS and Alex.

E

 

hi sbya,
Tidied the files.
Unzip for nets and asys.
E

 

hi papa,
I did try without the MODEL text, got this error , ref image.

I cannot see any differences in the remainder of the text/s, as posted by the TS and Alex.

E

That is because there is a fixed list of recognized models. The recognized models are listed on the HELP page for the .model statement. I'm pretty sure that name is not on the list.

There are 16 recognized names including NPN, PNP, and VDMOS

 

Hi everyone,
I was simulating a simple RC circuit to find it's frequency response using the following two third party Murata capacitor models GRM155C71H104JE19 and GRM155C71H103JE19 in the following circuit.
View attachment 237983

I received the following error message: Multiple instances of "C1" as shown:
View attachment 237984 View attachment 237985

Please guide me how to solve this unexpected behaviour. The simulation is attached to this question.

Thank You,
With Regards,
Srinjay Bhattacharya

There are two problems:

1. The .SUBCKT statement is incorrect.
incorrect = .MODEL SUBCKT GRM155C71H104JE19 C port1 port2
correct =.SUBCKT GRM155C71H104JE19 port1 port2


2. The symbol "Prefix" attribute is incorrect.
Since the component behavior is defined as a "subcircuit", as opposed to a "model", an "X" should be specified for the prefix attribute.

 

Hi everyone, I finally solved it thanks to the reply of Bordodynov. I'm summarizing it here:
1) I actually tried modifying the official spice model statements of the two capacitors which was a mistake creating a confusion between .SUBCKT and .MODEL files and also creating 3 terminals that I pointed out in one of my previous replies in this thread. Hence there is no need to modify the Spice model statements and stick to the original ones as provided by the manufacturer.

2) The main correction: while changing the value of the capacitor to the manufacturing name in the Component Attribute Editor, I missed adding an "x" to the value of the prefix "C1" in the same Component Attribute Editor and hence causing the error of Multiple instances of "C1". Hence, please don't forget to add "x" to the prefix else this problem will persist. Following are the snaps:

The mistake


The correction

I also attached both the error and no error(given by Bordodynov) files with this reply in case you want to further refer to them.

Thank You,
With Regards,
Srinjay Bhattacharya