Sparkgap model Spice ABM circuit netlist error message...

[nikv]

Greetings,

I am having a problem with modeling a Sparkgap in Multisim 11... refer attached ABM model circuit diagram... Sparkgap_ABM.ms11

I am using the Sparkgap_ABM model as a subcircuit in a component in another circuit... refer attached circuit diagram... Rev Limiter Coil Switcher.ms11

I created a netlist from the Sparkgap_ABM circuit... refer attached Spice subcircuit definition file... Sparkgap_ABM.cir

I used the Sparkgap_ABM.cir SPICE definition file to create the sparkgap component in the User Database Library which I used in the Rev Limiter Coil Switcher circuit.

When I run the simulation I get the following error message...

------ Checking SPICE netlist for Rev Limiter Coil Switcher - Sunday, May 13, 2012, 12:52:17 PM ------
SPICE Netlist Error in schematic RefDes 'v2', element 'bv2':  Element 'v1' referenced in expression does not exist in local scope or is not of a type compatible with the I() function
======= SPICE Netlist check completed, 1 error(s), 0 warning(s) =======
Error message from simulation: bv2:xx1: unknown controlling source v1
Error message from simulation: doAnalyses: No such parameter on this device
Error message from simulation: tran simulation(s) canceled

It appears to be related to the V1 voltage source that I am using in the Sparkgap_ABM circuit which I have set to 0V to act as a current sensor between nodes Pin1 and 3 and it is referenced in an equation used by V2 ABM Voltage source... I have checked all the SPICE definition criteria for using an ABM voltage source and I have changed the V1 definition statement to just vV1 pin1 3 0V from the more complex V source statement as shown in the Sparkgpa_ABM.cir file attached.  Does not seem to matter?

The sparkgap model works fine in MicroCap 9 and I am trying to port the model to Multisim...

I have run out of ideas as to what could be the problem and I suspect it is something unique to the way Multisim 11 processes Spice definition files...

I would much appreciate any suggestions from the members of this forum as to what could be causing this error?

[Tien_P · Accepted solution]

Hi Nikv,

I've looked at your Sparkga_abm circuit and there are two problems.

1.   In Multisim, if you want to use parameters in your equations, you have to put it in the Arbitrary SPICE Block, the SPICE engine will not see your parameters if you put it as text on the schematic.  Have a look at the attached circuit to see how to add parameters in Multisim.

2. In the ABM source V2, the last part of the equation is:  IF (ABS(I(V1))>Isus,10,10n)), you have to change V1 to VV1.  In Multisim, when you place a current or voltages source, Multisim automatically adds a V or I before the part reference.  If you select View>>SPICE netlist viewer, you can see circuit netlist as seen by SPICE engine.

[nikv]

Thank you very much for your assistance Tien.

That takes care of the Spice Netlist error...

Unfortunately now I have a convergence problem (timestep too small) and the convergence assistant could not help me... refering to the Help info on convergence problems I don't see what I can do with the circuit topology without altering the fundamental characteristics of the circuit I am trying to simulate and getting incorrect results???

I understand I am trying to simulate High Voltage fast changing transients and perhaps that is the problem but I am not sure... Microcap 9 is able to simulate the same circuit without any problems?

Perhaps you can suggest what I can do regarding the convergence problem?

I have attached revision 2 of the Sparkgap_ABM circuit and Revision 2 of the Coil Switcher circuit with some alterations to topology and component values.

Also attached is the Spice Netlist for the Sparkgap_ABM that I used as the model file for the sparkgap in the Coil Switcher circuit.

[nikv]

Some more information that may be of assistance regarding the convergence problem...

The model I used to create component U3, MJE5742 NPN Darlington power transistor used in the Coil switcher circuit I obtained from the ON Semiconductor website here...

http://www.onsemi.com/pub_link/Collateral/MJE5742.LIB

I have also attached this SPICE subcircuit model file...

[Tien_P]

Hi Nikv,

The Sparkgap_Abm circuit you created have a combination of SPICE and XSPICE models so you cannot create a  model from that circuit, you can only create a model from a circuit if all parts used in the circuit are SPICE base models.

I've merged both circuits to one page and I also replaced the 100V zeners with a model I found online.   I did get convergence problems but after I player around with the settings the circuit is now running.

If you were able to get this circuit to work on MicroCAP can you post the netlist from MicroCAP.  I could be that you are using different models.

[nikv]

Thank you kindly Tien... Good work 🙂

The output of the coil from your Multisim Circuit Transient Analysis almost looks like the MicroCap 9 transient analysis at the coil output... refer attached pdf file of the Microcap 9 Transient Analysis...

Except the Multisim circuit has too much ringing in the critical part of the waveform when the spark current is flowing, identified on the closeup of the coil output as the 796us region just after the High Voltage pulse drops from -16.6kV to -3.1kV after a few oscillations.

I managed to get the MicroCap Transient analysis to look almost exactly like a real Automotive Ignition coil and spark plug waveform...  with some tuning of coil and sparkgap parameters I think I can getter it even more representative of the real waveform.

Also attached you will find the Microcap 9 PSpice Coil Switcher circuit output and the Sparkgap model PSpice circuit output... I can also provide a Spice3 or HSPice output of the circuits from Microcap 9 if that is of any help to you?

[nikv]

The Microcap 9 Sparkgap circuit model has 2 parameters Vthres=10kV and Varc=2kV that set the Zener breakdown voltages I believe... not sure???

I could not figure out how to pass those parameters to an ideal Zener Model in Multisim so I just set them to 100V for test purposes.

Refer attachment of Microcap 9 Transient analysis coil output waveform v(19) closeup...

[edoering]

Thank you, Tien, your Point #2 cleared up a problem I would have taken hours to find otherwise!