AnsweredAssumed Answered

Incorrect SPICE file can cause HARBEC convergence failure

Question asked by ROB_LEFEBVRE Employee on May 31, 2005
We have had a recent case where HARBEC was not converging at DC.  It turns out that this was not a HARBEC problem at all, but was a problem with the device file supplied by a device manufacturer.

Normally, a SPICE file is supplied as a collection of .SUBCKT's and .MODEL's.  In contrast, the SPICE files supplied by a few manufacturers (and included with GENESYS) contain components not inside subcircuits.  The consequences of this problem are disastrous for any SPICE simulator (including HARBEC, which is based on SPICE in GENESYS 2004 and earlier).

A SPICE file trying to use an incorrect library file might look like this:

.INCLUDE device.lib
C1 5 3 50pF
Q1 4 3 1 transistor
V1 1 0 dc 10

This circuit apparently contains a capacitor, a voltage source and a transistor.  However, when SPICE includes the incorrect device.lib file, this becomes:

Q1  5 7 8 transistor
CCB 7 5 0.13E-12
LCX 5 2 0.10E-9
LEX 6 3 0.12E-9
.MODEL transistor NPN ...
C1 5 3 50pF
Q1 4 3 1 transistor
V1 1 0 dc 10

Notice that this has actually added components (including an additional transistor) to random nodes in the circuit!  Any simulator based on SPICE will suffer from this "problem".  In our initial library checks, we have found that some NEC and Philips transistors distributed with GENESYS suffer this problem.

Generally, this problem will be obvious and will result in non-convergence.  In any case, we strongly recommend that you be sure you have obtained the latest device models from the manufacturer before going into prototype or production stages.

Rob Lefebvre