Invalid subckt definition name

[jeffgies]

I've created a design and hunted down suitable models, but when I attempt to simulate, I get the following errors:

 ------ Checking SPICE netlist for DIB_channel - Tuesday, March 02, 2010, 2:30:36 PM ------
SPICE Netlist Error in schematic RefDes 'xmm1', element 'xmm1':  Invalid subckt definition name 'xxmm1_175423184'
SPICE Netlist Error in schematic RefDes 'xmm1', element '<unknown>':  Due to errors, the subckt instance 'xmm1' has been omitted from the simulation
SPICE Netlist Error in schematic RefDes 'd37', element 'xd37':  Invalid subckt definition name 'di_mmsz5254b__jgparts__1'
SPICE Netlist Error in schematic RefDes 'd37', element '<unknown>':  Due to errors, the subckt instance 'xd37' has been omitted from the simulation
SPICE Netlist Error in schematic RefDes 'd101', element 'dd101':  Unable to interpret 'di_s1jb__jgparts__2'
SPICE Netlist Error in schematic RefDes 'd5', element 'dd5':  Unable to interpret 'mmbd914lt1g__jgparts__1'
======= SPICE Netlist check completed, 6 error(s), 0 warning(s) =======

Someone else has reported a similar problem (http://forums.ni.com/ni/board/message?board.id=370&message.id=7182&query.id=1608889), but their problem was due to a space in the family name. I don't have spaces in any of the names I'm using.

Help!

[yyao · Accepted solution]

Hi there,

The root cause of this issue is your zener diode models have syntax errors. This is relatively easy to fix. Follow the following steps:

1. Double click on D37
2. Click on Edit Component in DB
3. Click on the Model tab
4. Click on Add/Edit
5. Add the following 1 line to the end of the model data text:
   .ends
6. Click Select (save and overwrite the old model)
7. Click OK (overwrite the old component)
8. Replace the diode with the new version that you just edited
9. Repeat for D69

The reason this works is the following. Every .subckt command must have a terminating .ends command. The zener diode models (which show up as DI_MMSZ5254B__JGPARTS__1 and DI_MMSZ5233B__JGPARTS__1 on my computer) have a .subckt but no .ends! You could see this for yourself. Click View>>SPICE Netlist Viewer. This is hiding all other models inside the zener diode model. When this happens, Multisim can't find the other models and you get your simulation error.

So, there you have it, the fix is quite simple. Just remember to copy SPICE models including the .subckt and the .ends lines next time.

Hope that helped!

[jeffgies]

Thanks Yi !!!

Jeff

[Zung]

Hi!

I have de same problem as him, but... I have the '.ends ' command:

------ Checking SPICE netlist for ModeloEL34Funcionando - miércoles, 07 de marzo de 2012, 21:34:56 ------
SPICE Netlist Error in schematic RefDes 'u1', element 'xu1': Unexpected '3' found on subckt instance line - too many nodes or parameter value missing name.
SPICE Netlist Error in schematic RefDes 'u1', element '<unknown>': Due to errors, the subckt instance 'xu1' has been omitted from the simulation
SPICE Netlist Error in schematic RefDes '', element 'x%p': Invalid subckt definition name '%m'
SPICE Netlist Error in schematic RefDes '', element '<unknown>': Due to errors, the subckt instance 'x%p' has been omitted from the simulation
======= SPICE Netlist check completed, 4 error(s), 0 warning(s) =======

I attach the circuit and the model code.

Could anyone have a look?... I'm a complete beginner and I'm having a lot of trouble with this.

Thanks for helping.

[Tien_P]

Hi Zung,

Your pin mapping table is incorrect.  Please have a look at the component tutorial from the following link, go to step 7, it explains the subcircuit statement for a SPICE model and how you mapped to symbol.

http://zone.ni.com/devzone/cda/tut/p/id/3173

THe model you are using only have 4 pins and this inforamtion came from this statement: .SUBCKT EL34 A S G K.  When you do the pin mapping in Multisim, it shoulb be like this:

[Zung]

Thank you for the explanation.

I have removed the unuseful pins, moreover it happened that I duplicated the pin information in the script. It was a complete mess.