Hello,

I have an error "ERROR(ORPSIM-16517): The fourth argument of the transistor in the netlist starts with a number"

does anybody know how to solve this problem?

thanks

 

It sounds like you are using a model whose fourth argument can't start with a number.

What kind of transistor are you using? What is the fourth argument for?

 

Hello, I have the same problem.

Here are the following models that present the same issue:

"The fourth argument of the transistor in the netlist starts with a number. If it is the substrate pin of a transistor, provide a model name. If it is a model, change the first character of the model name from number to an alphabet."

.MODEL 2SA1837 PNP (IS=2.39372559E-10 BF=300 NF=1.304015937 VAF=273 IKF=2.087725944 NK=0.94719458 ISE=1.46829699E-11 NE=1.526663542 BR=4 NR=1 VAR=20 IKR=1.05 RE=0 RB=1.8 RC=1.65 CJE=4.7407E-10 VJE=1.1 MJE=0.5 CJC=8.6700E-11 VJC=0.3 MJC=0.3 TF=1.642191E-09 FC=0.5 ITF=1.076260106 XTF=5.868994022 TR=1.38U )
.END

.model 2SA1943 PNP
+ IS=1.30E-10          BF=91.42             VAF=100
+ IKF=4.480            ISE=1.02E-10         NE=2.0
+ VAR=100              ISC=5.0900E-9        NC=1.5
+ BR=0.882             IKR=2.9015           RE=0.0011
+ RC=0.0553            RB=140.05            RBM=0.0041
+ IRB=8.5e-9           CJE=2.00E-10         FC=0.5
+ CJC=9.45E-10         VJC=0.48             MJC=0.28
+ TF=9.250E-10         XTF=10               VTF=10
+ ITF=1                TR=1.00E-8           EG=0.76
+ XTB=2.68             
.ends 2SA1943

.MODEL 2SC4793 NPN ( IS=1.8E-09 NF=1.43 BF=146.38 VAF=273 IKF=2.6 NK=0.95 ISE=6.286997E-10 NE=2.223629 BR=4 NR=1 VAR=20 IKR=1.05 RE=0 RB=1.7 RC=1.25 CJE=5.96964E-10 VJE=1.1 MJE=0.5 CJC=5.78E-11 VJC=0.3 MJC=0.3 TF=1.22678E-09 FC=0.5 ITF=10 XTF=99.52253015 TR=983N)
.END

.model 2SC5200 NPN
+ IS  = 3.0463E-11       BF  = 96.20           VAF = 100
+ IKF = 15.04256         ISE = 5.6190E-11      NE  = 2.0
+ BR  = 4.849            IKR = 1.05012         VAR = 100
+ ISC = 7.18E-8          NC  = 1.5             RE  = 0.0025
+ RB  = 20.18            RBM = 0.0014          IRB = 1.0E-7
+ RC  = 0.01137          CJE = 4.5000E-10      CJC = 8.4915E-10        
+ VJC = 0.68977          MJC = 0.54081         TF  = 6.8583E-10       
+ XTF = 9.5721           VTF = 10.425          ITF = 6.8697E-2       
+ TR  = 1.000E-8         XTB = 1.45            EG  = 0.82
+ FC  = 0.5
.ends 2SC5200

How do I can replace the first character of numerical parameters?

Does anyone have a clue?

Thanks,
Daniel.

 

Which simulation program do you use?

 

Cadence OrCAD Capture CIS 16.5-p003 (v16-5-13C)

Edit: They were .lib that I've imported via the Model Editor to .olb's

 

All this models work good in LTspice. All I did was add brackets to 2SC5200, 2SA1943. And LTspice don't like ".ends".

.model 2SA1943 PNP (
+ IS=1.30E-10          BF=91.42             VAF=100
+ IKF=4.480            ISE=1.02E-10         NE=2.0
+ VAR=100              ISC=5.0900E-9        NC=1.5
+ BR=0.882             IKR=2.9015           RE=0.0011
+ RC=0.0553            RB=140.05            RBM=0.0041
+ IRB=8.5e-9           CJE=2.00E-10         FC=0.5
+ CJC=9.45E-10         VJC=0.48             MJC=0.28
+ TF=9.250E-10         XTF=10               VTF=10
+ ITF=1                TR=1.00E-8           EG=0.76
+ XTB=2.68)            
.ends

.model 2SA1943 PNP (
+ IS=1.30E-10          BF=91.42             VAF=100
+ IKF=4.480            ISE=1.02E-10         NE=2.0
+ VAR=100              ISC=5.0900E-9        NC=1.5
+ BR=0.882             IKR=2.9015           RE=0.0011
+ RC=0.0553            RB=140.05            RBM=0.0041
+ IRB=8.5e-9           CJE=2.00E-10         FC=0.5
+ CJC=9.45E-10         VJC=0.48             MJC=0.28
+ TF=9.250E-10         XTF=10               VTF=10
+ ITF=1                TR=1.00E-8           EG=0.76
+ XTB=2.68 ).ends

 

Even after all recommended modifications I have the same error.

 

Try this

*---------------------------------------------------------------------
.MODEL KSC5200 NPN (IS=4.3031E-12 BF=152.1 NF=1.0 BR=6.155 NR=1.028
+ISE=1.3924E-11 NE=1.5 ISC=2.7542E-11 NC=1.95 VAF=60.0 VAR=6.51
+IKF=10.8637 IKR=0.1585 RB=2.47 RBM=0.02 IRB=0.08 RE=0.04 RC=0.015
+CJE=5.8111E-9 VJE=0.6506 MJE=0.3357 FC=0.5 CJC=6.4394E-10 VJC=0.5
+MJC=0.3966 XCJC=0.7624 XTB=1.0445 EG=1.1663 XTI=3.0
+RCO=0.21 GAMMA=10E-8)
*$
*--------------------------------------------------------
.MODEL KSA1943 PNP (IS=3.5476E-11 BF=159.9 NF=1.0 BR=25.75 NR=1.011
+    ISE=2.5119E-10 NE=2 ISC=7.9433E-11 NC=1.37 VAF=60.0 VAR=11.07 IKF=2.8370
+    IKR=0.3548 RB=2.74 RBM=0.0381 IRB=3.6308E-3 RE=0.06 RC=0.01 CJE=4.1783E-9
+    VJE=0.6354 MJE=0.3374 FC=0.5 CJC=1.1383E-9 VJC=0.5 MJC=0.3699 XCJC=0.7624    
+    XTB=1.5306 EG=1.1751 XTI=3.0 RCO=0.21 GAMMA=10E-8)
*$
*-----------------------------------------------------

 

The same error persists, weird thing.

Thank you.

 

I have a solution!!!!!!!!!

Oh god, finally, after 2 weeks.

The solution is under edit simulation profile -> configuration files

browse for nom.lib at default library folder if it isn't there and make it global.

Also, do this for your custom made libraries, but you don't need to make them global, just add to the project.

This will fix the problem.

Thanks for all the help, I hope this thread helps someone with same problems in the future.