MMBTA64 model problem, can I use a pnp BJT model? How to boost (set) hf?

Schematic Simulation (Ngspice)
1

I want to simulate a circuit including an MMBTA64 PNP darlington transistor. Any approximation will work for me, but I do need a high hf, the MMBTA64 has 20.000.

The model provided by DIODES:

*SRC=MMBTA64;DI_MMBTA64;BJTs PNP;Darlington;30.0V 0.500A Diodes Inc.  Darlington Transistor
*SYM=DARBJTP
.SUBCKT DII_MMBTA64 col base emtr
Q1 col base eb QPWR .1
Q2 col eb emtr QPWR
D1  col emtr DSUB
D2 base eb DSUB
.MODEL QPWR PNP  (IS=600f NF=1.00 BF=141  VAF=98.6
+ IKF=0.400 ISE=34.6p NE=2.00 BR=4.00 NR=1.00
+ VAR=40.0  IKR=0.600 RE=0.340 RB=1.36  RC=0.136
+ XTB=1.5 CJE=115p  VJE=0.740 MJE=0.450 CJC=16.5p
+  VJC=1.10 MJC=0.240 TF=3.57n  TR=614n )

lacked .ENDS at the end, which I added.
The in simulation, I get error messages:

warning, can’t find model ‘dsub’ from line
d1 col emtr dsub
warning, can’t find model ‘dsub’ from line
d2 base eb dsub

Error on line 22 or its substitute:
d.xt1.d1 nc-t1-0 nc-t1-2 dsub
could not find a valid modelname

which go away when I exclude the darlington from the simulation.

I would be happy to use a standard PNP model, but can I set parameters to mimick the high hf? I do not recognise (nor have any knowledge about) the parameters that one can set in the standard BJT PNP model.

Thanks,
Jan

2

In the MMBTA 13 model they add:

.MODEL DSUB D( IS=360f N=1 RS=4.00  BV=30.0 
+ IBV=.001  CJO=13.9p TT=617n ) 
.ENDS

and in the MMBTA14 model

.MODEL DSUB D( IS=360f N=1 RS=0.333  BV=30.0
+ IBV=.001  CJO=13.9p TT=614n )

so I guess such a definition is also needed here, but with what values (for RS?)

3

If you look at your two posts, you will see that the text processor has mangled your model descriptions. Please edit your posts and mark this text (the models) as pre-formatted text.

Concerning the models for DSUB: The selection is probably uncritical, as they describe the (internal) diodes which are reverse baised under normal operation. So RS is not that important, and of course we don’t know the exact value.

You may approach Diodes Inc. and ask them for an bug free model.

Another small issue: ngspice requires m=0.1. Without m there would be a warning and then the fact ignored, that this transistor is smaller by a factor of 10.

*SRC=MMBTA64;DI_MMBTA64;BJTs PNP;Darlington;30.0V 0.500A Diodes Inc.  Darlington Transistor
*SYM=DARBJTP
.SUBCKT DII_MMBTA64 col base emtr
Q1 col base eb QPWR m=.1
Q2 col eb emtr QPWR
D1  col emtr DSUB
D2 base eb DSUB
.MODEL QPWR PNP  (IS=600f NF=1.00 BF=141  VAF=98.6
+ IKF=0.400 ISE=34.6p NE=2.00 BR=4.00 NR=1.00
+ VAR=40.0  IKR=0.600 RE=0.340 RB=1.36  RC=0.136
+ XTB=1.5 CJE=115p  VJE=0.740 MJE=0.450 CJC=16.5p
+  VJC=1.10 MJC=0.240 TF=3.57n  TR=614n )
.MODEL DSUB D( IS=360f N=1 RS=4.00  BV=30.0 
+ IBV=.001  CJO=13.9p TT=617n ) 
.ENDS
4

Thanks Holger, but this still gives the following error messages:

Warning: redefinition of .subckt dii_mmbta64, ignored
warning, can’t find model ‘dsub’ from line
d1 col emtr dsub
warning, can’t find model ‘dsub’ from line
d2 base eb dsub
Circuit: KiCad schematic
Error on line 22 or its substitute:
d.xt1.d1 probe_int_probe_int_nc-t1-0_xt1_1_xt1_1 probe_int_probe_int_nc-t1-2_xt1_3_xt1_3 dsub
could not find a valid modelname
Error: circuit not parsed.

5

This sound like you now have two models with the same name .subckt dii_mmbta64. The first one probably is the defect one, the second is ignored, therefore the warning.

You should not add the new model, but replace the old one.