topic Error Message Simulation in EAGLE Forum

Error Message Simulation

tvk.rohrhofer — Wed, 17 Aug 2022 07:12:33 GMT

Hi guys,

Does somebody know something about these errors?

Betreff: Error Message Simulation

holger.vogt — Wed, 17 Aug 2022 09:13:23 GMT

You have sent a token "RATIO" to ngspice, which is not defined. Thus ngspice does not understand it and bails out.

Please check your circuit for "RATIO".

Betreff: Error Message Simulation

tvk.rohrhofer — Wed, 17 Aug 2022 11:03:06 GMT

What is "RATIO"?

Betreff: Error Message Simulation

holger.vogt — Wed, 17 Aug 2022 11:43:44 GMT

That's exactly the question.

Please post the Simulation Results --> Netlist here.

Betreff: Error Message Simulation

tvk.rohrhofer — Wed, 17 Aug 2022 11:46:25 GMT

That's the Netlist

* SpiceNetList
*
* Exported from Str.Laufplan_Lichtschranke-Test.sch at 17.08.2022 13:47
*
* EAGLE Version 9.6.2 Copyright (c) 1988-2020 Autodesk, Inc.
*
.TEMP=25.0

* --------- .OPTIONS ---------
.OPTIONS ABSTOL=1e-12 GMIN=1e-12 PIVREL=1e-3 ITL1=100 ITL2=50 PIVTOL=1e-13 RELTOL=1e-3 VNTOL=1e-6 CHGTOL=1e-15 ITL4=10 METHOD=TRAP SRCSTEPS=0 TRTOL=7 NODE

* --------- .PARAMS ---------

* --------- devices ---------
R_R3 N_4 N_3 100k
L_T2 0 N_3 PFET
R_R1 N_2 N_5 1k
B_V1 N_5 0 9V
R_R2 N_3 N_5 47k
Q_Q1 N_4 N_5 N_6 QNPN
D_D2 0 N_2 DMOD
D_LED1 0 N_6 DMOD

* --------- models ---------

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/DMOD.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic diode intrinsic model
**********************
.MODEL DMOD D

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/PFET.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic pfet intrinsic model
**********************
.MODEL PFET PMOS (LEVEL=3)

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/QNPN.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic npn intrinsic model
**********************
.MODEL QNPN NPN

* --------- simulation ---------
.control
set filetype=ascii
DC V_V1 9 0 -0.018
write Str.Laufplan_Lichtschranke-Test.sch.sim I(B_V1)
.endc

.END

Betreff: Error Message Simulation

holger.vogt — Wed, 17 Aug 2022 11:59:04 GMT

The netlist does not contain "RATIO". Different netlist?

The netlist above shows two errors (in recent ngspice-37):

warning, model type mismatch in line l_t2 0 n_3 pfet ERROR: mal formed B line: b_v1 n_5 0 9v

Line

L_T2 0 N_3 PFET

starts with an L. So it is not a MOSFET, but an inductor.

Line

B_V1 N_5 0 9V

is wrong, it should be a voltage source like

V_V1 N_5 0 9V

Please check your circuit and the attached models.

Betreff: Error Message Simulation

tvk.rohrhofer — Wed, 17 Aug 2022 12:06:44 GMT

I am very sorry but I send the wrong netlist. That's the right one.

* SpiceNetList
*
* Exported from Str.Laufplan_Lichtschranke.sch at 17.08.2022 14:07
*
* EAGLE Version 9.6.2 Copyright (c) 1988-2020 Autodesk, Inc.
*
.TEMP=25.0

* --------- .OPTIONS ---------
.OPTIONS ABSTOL=1e-12 GMIN=1e-12 PIVREL=1e-3 ITL1=100 ITL2=50 PIVTOL=1e-13 RELTOL=1e-3 VNTOL=1e-6 RSHUNT=10e9 CHGTOL=1e-15 ITL4=10 METHOD=TRAP SRCSTEPS=0 TRTOL=7 NODE

* --------- .PARAMS ---------

* --------- devices ---------
X_K1 N_7 N_9 0 N_6 XFORMER
R_R3 N_4 N_3 100k
R_R1 N_2 N_1 1k
V_V1 N_5 0 DC 0V AC 9V
D_T1 0 N_3 PFET
R_R4 N_9 0 100k
V_V2 N_7 0 DC 9V AC 0
R_R2 N_3 N_1 47k
Q_Q1 N_4 N_1 N_6 QNPN
D_D2 N_5 N_1 DMOD
C_C2 N_6 0 22µ/35V
D_D1 0 N_2 DMOD

* --------- models ---------

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/DMOD.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic diode intrinsic model
**********************
.MODEL DMOD D

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/PFET.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic pfet intrinsic model
**********************
.MODEL PFET PMOS (LEVEL=3)

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/QNPN.mdl
**********************
* Autodesk EAGLE - Spice Model File
* Date: 9/17/17
* basic npn intrinsic model
**********************
.MODEL QNPN NPN

* model file: C:/Users/TiVi/OneDrive/Documents/EAGLE/spice/XFORMER.mdl
**********************
* Autodesk EAGLE - Spice Model File
* transformer subcircuit, requires RATIO parameter defined
* Date: 10/1/17
**********************
.SUBCKT XFORMER 1 2 3 4
E 5 4 1 2 {RATIO}
F 1 2 VM {RATIO}
VM 5 6
RP 1 2 1MEG
RS 6 3 1U
.ENDS XFORMER

* --------- simulation ---------

.control
set filetype=ascii
TRAN 0.1 50 0 0.1
write Str.Laufplan_Lichtschranke.sch.sim I(V_V2) I(V_V1)
.endc

.END

Betreff: Error Message Simulation

holger.vogt — Wed, 17 Aug 2022 12:56:47 GMT

Still two bugs:

D_T1 0 N_3 PFET

calls for a MOSFET model (PFET), but line starts with D (which is a diode).

Transformer model XFORMER states

* transformer subcircuit, requires RATIO parameter defined

(see netlist above).

There is no definition of the RATIO parameter in the netlist, something like:

.param RATIO = 5

Betreff: Error Message Simulation

tvk.rohrhofer — Wed, 17 Aug 2022 13:16:58 GMT

How can I get this ".param RATIO = 5" and the MOSFET in my netlist?

Betreff: Error Message Simulation

holger.vogt — Wed, 17 Aug 2022 16:14:03 GMT

Is there any example for the XFORMER in the examples section? I am quite convinced there is an example for adding a MOS device.

Unfortunately I do not use EAGLE for schematic entry, so cannot be of help here.

Re: Error Message Simulation

jorge_garcia — Wed, 17 Aug 2022 18:06:09 GMT

Hi @tvk.rohrhofer,

Here's the transformer example in EAGLE.

Here's the example, transformer file that ships with EAGLE.

Let me know if there's anything else I can do for you.

Best Regards,