Thread: [Ngspice-users] Transient solution fail with oscillator

Brought to you by: dwarning, h_vogt, nicolati, pnenzi

ngspice-users

[Ngspice-users] Transient solution fail with oscillator

From: Dominique M. <dom...@gm...> - 2018-10-19 12:13:50

Hi,

When running a simulation of a Clapp pentode oscillator with ngspice 28,
I get:

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Error: 0, -0.022 out of range for pwr
Note: Starting dynamic gmin stepping
Trying gmin =   1.0000E-03 Error: 0, -0.022 out of range for pwr
Warning: Further gmin increment
>snip>
Warning: Dynamic gmin stepping failed
Note: Starting source stepping
Supplies reduced to   0.0000% Error: 0, -0.022 out of range for pwr

Trying gmin =   1.0000E-02 Error: 0, -0.022 out of range for pwr
Warning: gmin step failed
Warning: source stepping failed

Transient solution failed -
<snip>
doAnalyses: iteration limit reached

tran simulation(s) aborted

###

The circuit is:

.SUBCKT EF89 1 2 3 4 ; A G2 G1 C;
X1 1 2 3 4 PenthodeVDE 
+ PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
1199.3
+ MUb=  7.8 EXb=0.978 svar= 0.068
+ Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
als=  2.07 RGI=2000
+ CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
.ENDS
****************************************************
.SUBCKT PenthodeVDE 1 2 3 4; A G2 G1 C
+ PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
1199.3
+ MUb=  7.8 EXb=0.978 svar= 0.068
+ Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
als=  2.07 RGI=2000
+ CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
RE1  7 0  1MEG    ; DUMMY SO NODE 7 HAS 2 CONNECTIONS
E1   7 0  VALUE=
+{V(2,4)/KP*LN(1+EXP(KP*(1/MU+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
E11 17 0  VALUE=
+{V(2,4)/KP*LN(1+EXP(KP*(1/MUb+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
E20  9 0  VALUE = {(1-svar)*0.5*(PWR(V(7),EX)+PWRS(V(7),EX))+
svar*0.5*(PWR(V(17),EXb)+PWRS(V(17),EXb))} E2   8 0 VALUE =
{Ookg1mOokG2 + Aokg1*V(1,4) -
alkg1palskg2*Exp(-be*V(1,4)*SQRT(be*V(1,4)))} G1   1 4  VALUE =
{V(9)*V(8)} G2   2 4 VALUE = {V(9)/KG2 *(1+als*Exp(-be*V(1,4) *
SQRT(be*V(1,4))))} RCP  1 4  1G      ; FOR CONVERGENCE	A  - C
C1   3 4  {CCG1}   ; CATHODE-GRID 1	C  - G1 C4   2 4  {CCG2}   ;
CATHODE-GRID 2	C  - G2 C5   2 3  {CG1G2}   ; GRID 1 -GRID
2	G1  - G2 C2   1 3  {CPG1}  ; GRID 1-PLATE	G1 - A
C3   1 4  {CCP}   ; CATHODE-PLATE	A  - C
R1   3 5  {RGI}   ; FOR GRID CURRENT	G1 - 5
D3   5 4  DX      ; FOR GRID CURRENT	5  - C
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS PenthodeVDE
***************** Main circuit
Rbias 6 sortie 2.7k  
Cbias 6 sortie 3.3n  
X1 1 1 grille 6 EF89
RL2 5 0 8.1  
Rconv 0 3 1e12  
L2 sortie 5 0.00163 
C1 2 sortie 680p  
C2 sortie 0 680p  
Ro 4 2 4.6  
Lo 4 3 100u 
Co 0 3 345p
C3 2 grille 100p  
Rg grille 0 1e6  
VG1 1 0 DC 158V
.INCLUDE Simulation.cmd
.end

Simulation.cmd:

.INCLUDE ~/Elec/work/ngspice/pspice.alias
.control
	TRAN 1u 5m
	plot v(sortie) v(grille)
.endc

pspice.alias:
.func LIMIT(x,a,b) {min(max(x, a), b)}
.func PWR(x,a) {abs(x) ** a}
.func PWRS(x,a) {sgn(x) * PWR(x,a)}
.func stp(x) {u(x)}

I try to run the same circuit and simulation using an ECC85/6AQ8 valve
with another Ayumi's model, and it work fine with it:
.SUBCKT 6AQ8 A G K
BGG   GG   0 V=V(G,K)+0.46274
BM1   M1   0 V=(0.016397559*(URAMP(V(A,K))+1e-10))**-1.8244468
BM2   M2   0
V=(0.4512029*(URAMP(V(GG)+URAMP(V(A,K))/33.468219)+1e-10))**3.3244468
BP    P    0
V=0.0053412983*(URAMP(V(GG)+URAMP(V(A,K))/74.175541)+1e-10)**1.5 BIK
IK   0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0076348*V(M1)*V(M2) BIG   IG   0
V=0.0026706491*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+0.4)
BIAK  A    K
I=URAMP(V(IK,IG)-URAMP(V(IK,IG)-(0.0027790257*URAMP(V(A,K))**1.5)))+1e-10*V(A,K)
BIGK  G    K I=V(IG)
* CAPS
CGA   G    A 1.5p
CGK   G    K 3.1p
CAK   A    K 1.2p
.ENDS

I am a little bit lost here. What can I do to make that oscillator to
run with that f. EF89 pentode model? It work on the bench with both
valves.

Best,
Dominique


-- 
If you have a problem and you are not doing anything to fix it, you are
at the heart of the problem.

Re: [Ngspice-users] Transient solution fail with oscillator

From: <mh...@ia...> - 2018-10-19 19:40:21

Attachments: clapp.eps

On 2018-10-19 14:15, Dominique Michel wrote:
[..]
> I try to run the same circuit and simulation using an ECC85/6AQ8 valve
> with another Ayumi's model, and it work fine with it:
[..]
> I am a little bit lost here. What can I do to make that oscillator to
> run with that f. EF89 pentode model? It work on the bench with both
> valves.

That model and its default parameters has too many flaws to list here.
It exposed a latent problem in my Koren.lib ( the argument of LOG(x)
should be positive ), and I thank you for bringing that to my attention.

Try the below, it oscillates at ~5 MHz with les than 0.5% of THD.

-marcel

~~~
.TITLE Clapp oscillator

.func limpow(x,y) { (x <= 0) ? 0  : 2*PWR(x,y) }
.func plog(x)   { (x <= 0) ? 1u : log(x) }

******************
.subckt pentode1 1 2 3 4 MU=9.98 EX=0.944 KG1=165.6 KG2=4500 KP=38.07 
KVB=35.4 VCT=0 RGI=1000 CCG=14p CPG1=0.8p CCP=12p $ A G2 G1 C
RE1  7 0  1MEG    $ dummy so node 7 has 2 connections
E1   7 0  value = { v(2,4)/kp*plog(1+exp((1/mu+v(3,4)/v(2,4))*kp)) } $ 
E1 breaks up long equation for g1.
G1   1 4  value = { limpow(v(7),ex)/kg1*atan(v(1,4)/kvb) }
G2   2 4  value = { (exp(ex*(plog((v(2,4)/mu)+v(3,4)))))/kg2 }
RCP  1 4  1G      $ for convergence	A  - C
C1   3 4  {ccg}   $ cathode-grid 1	C  - G1
C2   1 3  {cpg1}  $ grid 1-plate	G1 - A
C3   1 4  {ccp}   $ cathode-plate	A  - C
R1   3 5  {rgi}   $ for grid current	G1 - 5
D3   5 4  DX      $ for grid current	5  - C
.ends pentode1

******************
.SUBCKT EF89  1 2 3 4 		$ A G2 G1 C (Pentode)
* La Radiotechnique AKA 6DA6
X1 1 2 3 4 PENTODE1 MU=30.52 EX=1.350 KG1=926.7 KG2=4500 KP=39.49 
KVB=23.6 VCT=0.00 RGI=2000 CCG=5.5p CPG1=0.0p CCP=5.1p
.ENDS EF89

*****************
* Main circuit
Rbias 6      sortie 2.7k
Cbias 6      sortie 3.3n
X1    1      1      grille 6  EF89
RL2   5      0      8.1
Rconv 0      3      1e12
L2    sortie 5      0.00163
C1    2      sortie 680p
C2    sortie 0      680p
Ro    4      2      4.6
Lo    4      3      100u
Co    0      3      345p
C3    2      grille 100p
Rg    grille 0      1e6
VG1   1      0      DC=158V

.control
	listing e
	TRAN 5n 200u 0 5n UIC
	write clapp.raw
	plot v(sortie)
	rusage all
.endc

.END
~~~

Re: [Ngspice-users] Transient solution fail with oscillator

From: Dominique M. <dom...@gm...> - 2018-10-20 10:33:39

Le Fri, 19 Oct 2018 21:40:10 +0200,
mh...@ia... a écrit :

> On 2018-10-19 14:15, Dominique Michel wrote:
> [..]
> > I try to run the same circuit and simulation using an ECC85/6AQ8
> > valve with another Ayumi's model, and it work fine with it:  
> [..]
> > I am a little bit lost here. What can I do to make that oscillator
> > to run with that f. EF89 pentode model? It work on the bench with
> > both valves.  
> 
> That model and its default parameters has too many flaws to list here.
> It exposed a latent problem in my Koren.lib ( the argument of LOG(x)
> should be positive ), and I thank you for bringing that to my
> attention.
I get troubles with all existing vacuum tubes models. The only one
which both run fine and is electrically correct is the diode model from
Perugini. More grids you add, more complicated, harder to run and more
approximative become the models.

> 
> Try the below, it oscillates at ~5 MHz with les than 0.5% of THD.

Thank you, it work fine. Just the DX model is missing, but I took it
from the other EF89 model.

Dominique

> 
> -marcel
> 
> ~~~
> .TITLE Clapp oscillator
> 
> .func limpow(x,y) { (x <= 0) ? 0  : 2*PWR(x,y) }
> .func plog(x)   { (x <= 0) ? 1u : log(x) }
> 
> ******************
> .subckt pentode1 1 2 3 4 MU=9.98 EX=0.944 KG1=165.6 KG2=4500 KP=38.07 
> KVB=35.4 VCT=0 RGI=1000 CCG=14p CPG1=0.8p CCP=12p $ A G2 G1 C
> RE1  7 0  1MEG    $ dummy so node 7 has 2 connections
> E1   7 0  value = { v(2,4)/kp*plog(1+exp((1/mu+v(3,4)/v(2,4))*kp)) }
> $ E1 breaks up long equation for g1.
> G1   1 4  value = { limpow(v(7),ex)/kg1*atan(v(1,4)/kvb) }
> G2   2 4  value = { (exp(ex*(plog((v(2,4)/mu)+v(3,4)))))/kg2 }
> RCP  1 4  1G      $ for convergence	A  - C
> C1   3 4  {ccg}   $ cathode-grid 1	C  - G1
> C2   1 3  {cpg1}  $ grid 1-plate	G1 - A
> C3   1 4  {ccp}   $ cathode-plate	A  - C
> R1   3 5  {rgi}   $ for grid current	G1 - 5
> D3   5 4  DX      $ for grid current	5  - C
> .ends pentode1
> 
> ******************
> .SUBCKT EF89  1 2 3 4 		$ A G2 G1 C (Pentode)
> * La Radiotechnique AKA 6DA6
> X1 1 2 3 4 PENTODE1 MU=30.52 EX=1.350 KG1=926.7 KG2=4500 KP=39.49 
> KVB=23.6 VCT=0.00 RGI=2000 CCG=5.5p CPG1=0.0p CCP=5.1p
> .ENDS EF89
> 
> *****************
> * Main circuit
> Rbias 6      sortie 2.7k
> Cbias 6      sortie 3.3n
> X1    1      1      grille 6  EF89
> RL2   5      0      8.1
> Rconv 0      3      1e12
> L2    sortie 5      0.00163
> C1    2      sortie 680p
> C2    sortie 0      680p
> Ro    4      2      4.6
> Lo    4      3      100u
> Co    0      3      345p
> C3    2      grille 100p
> Rg    grille 0      1e6
> VG1   1      0      DC=158V
> 
> .control
> 	listing e
> 	TRAN 5n 200u 0 5n UIC
> 	write clapp.raw
> 	plot v(sortie)
> 	rusage all
> .endc
> 
> .END
> ~~~


-- 
If you have a problem and you are not doing anything to fix it, you are
at the heart of the problem.

Re: [Ngspice-users] Transient solution fail with oscillator

From: Tom <mad...@go...> - 2018-10-20 11:13:57

Sometimes adding some sensible initial conditions can help in a 
situation like this - set one of the grids to a max or min value 
expected during oscillation.
Tom

On 19/10/2018 13:15, Dominique Michel wrote:
> Hi,
>
> When running a simulation of a Clapp pentode oscillator with ngspice 28,
> I get:
>
> Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
>
> Error: 0, -0.022 out of range for pwr
> Note: Starting dynamic gmin stepping
> Trying gmin =   1.0000E-03 Error: 0, -0.022 out of range for pwr
> Warning: Further gmin increment
>> snip>
> Warning: Dynamic gmin stepping failed
> Note: Starting source stepping
> Supplies reduced to   0.0000% Error: 0, -0.022 out of range for pwr
>
> Trying gmin =   1.0000E-02 Error: 0, -0.022 out of range for pwr
> Warning: gmin step failed
> Warning: source stepping failed
>
> Transient solution failed -
> <snip>
> doAnalyses: iteration limit reached
>
> tran simulation(s) aborted
>
> ###
>
> The circuit is:
>
> .SUBCKT EF89 1 2 3 4 ; A G2 G1 C;
> X1 1 2 3 4 PenthodeVDE
> + PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
> 1199.3
> + MUb=  7.8 EXb=0.978 svar= 0.068
> + Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
> als=  2.07 RGI=2000
> + CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
> .ENDS
> ****************************************************
> .SUBCKT PenthodeVDE 1 2 3 4; A G2 G1 C
> + PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
> 1199.3
> + MUb=  7.8 EXb=0.978 svar= 0.068
> + Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
> als=  2.07 RGI=2000
> + CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
> RE1  7 0  1MEG    ; DUMMY SO NODE 7 HAS 2 CONNECTIONS
> E1   7 0  VALUE=
> +{V(2,4)/KP*LN(1+EXP(KP*(1/MU+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
> E11 17 0  VALUE=
> +{V(2,4)/KP*LN(1+EXP(KP*(1/MUb+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
> E20  9 0  VALUE = {(1-svar)*0.5*(PWR(V(7),EX)+PWRS(V(7),EX))+
> svar*0.5*(PWR(V(17),EXb)+PWRS(V(17),EXb))} E2   8 0 VALUE =
> {Ookg1mOokG2 + Aokg1*V(1,4) -
> alkg1palskg2*Exp(-be*V(1,4)*SQRT(be*V(1,4)))} G1   1 4  VALUE =
> {V(9)*V(8)} G2   2 4 VALUE = {V(9)/KG2 *(1+als*Exp(-be*V(1,4) *
> SQRT(be*V(1,4))))} RCP  1 4  1G      ; FOR CONVERGENCE	A  - C
> C1   3 4  {CCG1}   ; CATHODE-GRID 1	C  - G1 C4   2 4  {CCG2}   ;
> CATHODE-GRID 2	C  - G2 C5   2 3  {CG1G2}   ; GRID 1 -GRID
> 2	G1  - G2 C2   1 3  {CPG1}  ; GRID 1-PLATE	G1 - A
> C3   1 4  {CCP}   ; CATHODE-PLATE	A  - C
> R1   3 5  {RGI}   ; FOR GRID CURRENT	G1 - 5
> D3   5 4  DX      ; FOR GRID CURRENT	5  - C
> .MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
> .ENDS PenthodeVDE
> ***************** Main circuit
> Rbias 6 sortie 2.7k
> Cbias 6 sortie 3.3n
> X1 1 1 grille 6 EF89
> RL2 5 0 8.1
> Rconv 0 3 1e12
> L2 sortie 5 0.00163
> C1 2 sortie 680p
> C2 sortie 0 680p
> Ro 4 2 4.6
> Lo 4 3 100u
> Co 0 3 345p
> C3 2 grille 100p
> Rg grille 0 1e6
> VG1 1 0 DC 158V
> .INCLUDE Simulation.cmd
> .end
>
> Simulation.cmd:
>
> .INCLUDE ~/Elec/work/ngspice/pspice.alias
> .control
> 	TRAN 1u 5m
> 	plot v(sortie) v(grille)
> .endc
>
> pspice.alias:
> .func LIMIT(x,a,b) {min(max(x, a), b)}
> .func PWR(x,a) {abs(x) ** a}
> .func PWRS(x,a) {sgn(x) * PWR(x,a)}
> .func stp(x) {u(x)}
>
> I try to run the same circuit and simulation using an ECC85/6AQ8 valve
> with another Ayumi's model, and it work fine with it:
> .SUBCKT 6AQ8 A G K
> BGG   GG   0 V=V(G,K)+0.46274
> BM1   M1   0 V=(0.016397559*(URAMP(V(A,K))+1e-10))**-1.8244468
> BM2   M2   0
> V=(0.4512029*(URAMP(V(GG)+URAMP(V(A,K))/33.468219)+1e-10))**3.3244468
> BP    P    0
> V=0.0053412983*(URAMP(V(GG)+URAMP(V(A,K))/74.175541)+1e-10)**1.5 BIK
> IK   0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0076348*V(M1)*V(M2) BIG   IG   0
> V=0.0026706491*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+0.4)
> BIAK  A    K
> I=URAMP(V(IK,IG)-URAMP(V(IK,IG)-(0.0027790257*URAMP(V(A,K))**1.5)))+1e-10*V(A,K)
> BIGK  G    K I=V(IG)
> * CAPS
> CGA   G    A 1.5p
> CGK   G    K 3.1p
> CAK   A    K 1.2p
> .ENDS
>
> I am a little bit lost here. What can I do to make that oscillator to
> run with that f. EF89 pentode model? It work on the bench with both
> valves.
>
> Best,
> Dominique
>
>

Re: [Ngspice-users] Transient solution fail with oscillator

From: Dominique M. <dom...@gm...> - 2018-10-21 09:16:24

Le Sat, 20 Oct 2018 12:13:45 +0100,
Tom via Ngspice-users <ngs...@li...> a écrit :

> Sometimes adding some sensible initial conditions can help in a 
> situation like this - set one of the grids to a max or min value 
> expected during oscillation.
> Tom

When playing with the components values and using the Ayumi triode
model (as well than other simulations with other models like Koren), it
can append the oscillation start, but after some time, in the
stabilization phase of the oscillation, it just fail to converge or
take forever. The pentode Koren model from Marcel seam to run well
with that simulation.

Otherwise the result is not bad with the exception of the AC voltages
being too high in comparison with the montage on the bench. I am in
the way to make a theremin with it, from an old valve radio. 

But to see how the oscillator react with parameters changes, it is
perfect. I make videos with the analysis results.

Best,
Dominique

> 
> On 19/10/2018 13:15, Dominique Michel wrote:
> > Hi,
> >
> > When running a simulation of a Clapp pentode oscillator with
> > ngspice 28, I get:
> >
> > Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
> >
> > Error: 0, -0.022 out of range for pwr
> > Note: Starting dynamic gmin stepping
> > Trying gmin =   1.0000E-03 Error: 0, -0.022 out of range for pwr
> > Warning: Further gmin increment  
> >> snip>  
> > Warning: Dynamic gmin stepping failed
> > Note: Starting source stepping
> > Supplies reduced to   0.0000% Error: 0, -0.022 out of range for pwr
> >
> > Trying gmin =   1.0000E-02 Error: 0, -0.022 out of range for pwr
> > Warning: gmin step failed
> > Warning: source stepping failed
> >
> > Transient solution failed -
> > <snip>
> > doAnalyses: iteration limit reached
> >
> > tran simulation(s) aborted
> >
> > ###
> >
> > The circuit is:
> >
> > .SUBCKT EF89 1 2 3 4 ; A G2 G1 C;
> > X1 1 2 3 4 PenthodeVDE
> > + PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
> > 1199.3
> > + MUb=  7.8 EXb=0.978 svar= 0.068
> > + Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
> > als=  2.07 RGI=2000
> > + CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
> > .ENDS
> > ****************************************************
> > .SUBCKT PenthodeVDE 1 2 3 4; A G2 G1 C
> > + PARAMS: MU= 25.0 EX=1.418 kG1= 328.3 KP=  58.8 kVB =     0.0 kG2=
> > 1199.3
> > + MUb=  7.8 EXb=0.978 svar= 0.068
> > + Ookg1mOokG2=.22E-02 Aokg1=.36E-06 alkg1palskg2=.22E-02 be= 0.122
> > als=  2.07 RGI=2000
> > + CCG1=5.5P  CCG2 = 0.0p CPG1 = 0.002p  CG1G2 = 0.0p CCP=5.1P  ;
> > RE1  7 0  1MEG    ; DUMMY SO NODE 7 HAS 2 CONNECTIONS
> > E1   7 0  VALUE=
> > +{V(2,4)/KP*LN(1+EXP(KP*(1/MU+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
> > E11 17 0  VALUE=
> > +{V(2,4)/KP*LN(1+EXP(KP*(1/MUb+V(3,4)/SQRT(KVB+V(2,4)*V(2,4)))))}
> > E20  9 0  VALUE = {(1-svar)*0.5*(PWR(V(7),EX)+PWRS(V(7),EX))+
> > svar*0.5*(PWR(V(17),EXb)+PWRS(V(17),EXb))} E2   8 0 VALUE =
> > {Ookg1mOokG2 + Aokg1*V(1,4) -
> > alkg1palskg2*Exp(-be*V(1,4)*SQRT(be*V(1,4)))} G1   1 4  VALUE =
> > {V(9)*V(8)} G2   2 4 VALUE = {V(9)/KG2 *(1+als*Exp(-be*V(1,4) *
> > SQRT(be*V(1,4))))} RCP  1 4  1G      ; FOR CONVERGENCE	A  - C
> > C1   3 4  {CCG1}   ; CATHODE-GRID 1	C  - G1 C4   2 4
> > {CCG2}   ; CATHODE-GRID 2	C  - G2 C5   2 3  {CG1G2}   ; GRID
> > 1 -GRID 2	G1  - G2 C2   1 3  {CPG1}  ; GRID 1-PLATE
> > G1 - A C3   1 4  {CCP}   ; CATHODE-PLATE	A  - C
> > R1   3 5  {RGI}   ; FOR GRID CURRENT	G1 - 5
> > D3   5 4  DX      ; FOR GRID CURRENT	5  - C
> > .MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
> > .ENDS PenthodeVDE
> > ***************** Main circuit
> > Rbias 6 sortie 2.7k
> > Cbias 6 sortie 3.3n
> > X1 1 1 grille 6 EF89
> > RL2 5 0 8.1
> > Rconv 0 3 1e12
> > L2 sortie 5 0.00163
> > C1 2 sortie 680p
> > C2 sortie 0 680p
> > Ro 4 2 4.6
> > Lo 4 3 100u
> > Co 0 3 345p
> > C3 2 grille 100p
> > Rg grille 0 1e6
> > VG1 1 0 DC 158V
> > .INCLUDE Simulation.cmd
> > .end
> >
> > Simulation.cmd:
> >
> > .INCLUDE ~/Elec/work/ngspice/pspice.alias
> > .control
> > 	TRAN 1u 5m
> > 	plot v(sortie) v(grille)
> > .endc
> >
> > pspice.alias:
> > .func LIMIT(x,a,b) {min(max(x, a), b)}
> > .func PWR(x,a) {abs(x) ** a}
> > .func PWRS(x,a) {sgn(x) * PWR(x,a)}
> > .func stp(x) {u(x)}
> >
> > I try to run the same circuit and simulation using an ECC85/6AQ8
> > valve with another Ayumi's model, and it work fine with it:
> > .SUBCKT 6AQ8 A G K
> > BGG   GG   0 V=V(G,K)+0.46274
> > BM1   M1   0 V=(0.016397559*(URAMP(V(A,K))+1e-10))**-1.8244468
> > BM2   M2   0
> > V=(0.4512029*(URAMP(V(GG)+URAMP(V(A,K))/33.468219)+1e-10))**3.3244468
> > BP    P    0
> > V=0.0053412983*(URAMP(V(GG)+URAMP(V(A,K))/74.175541)+1e-10)**1.5 BIK
> > IK   0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0076348*V(M1)*V(M2) BIG
> > IG   0
> > V=0.0026706491*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+0.4)
> > BIAK  A    K
> > I=URAMP(V(IK,IG)-URAMP(V(IK,IG)-(0.0027790257*URAMP(V(A,K))**1.5)))+1e-10*V(A,K)
> > BIGK  G    K I=V(IG)
> > * CAPS
> > CGA   G    A 1.5p
> > CGK   G    K 3.1p
> > CAK   A    K 1.2p
> > .ENDS
> >
> > I am a little bit lost here. What can I do to make that oscillator
> > to run with that f. EF89 pentode model? It work on the bench with
> > both valves.
> >
> > Best,
> > Dominique
> >
> >  
> 
> 
> 
> _______________________________________________
> Ngspice-users mailing list
> Ngs...@li...
> https://lists.sourceforge.net/lists/listinfo/ngspice-users


-- 
If you have a problem and you are not doing anything to fix it, you are
at the heart of the problem.

Re: [Ngspice-users] Transient solution fail with oscillator

From: Holger V. <hol...@un...> - 2018-10-21 10:08:01

Attachments: EF89-181020.cir

Adding some damping, increasing the time resolution, and adding the ABS 
function to every square root yields some results (Simulated with the 
rdecent Master Branch of ngspice, adding 'set ngbehavior=ltpsa' to 
.spiceinit)

Re: [Ngspice-users] Transient solution fail with oscillator

From: Dominique M. <dom...@gm...> - 2018-10-28 15:47:26

Le Sun, 21 Oct 2018 12:07:49 +0200,
Holger Vogt <hol...@un...> a écrit :

> Adding some damping, increasing the time resolution, and adding the
> ABS function to every square root yields some results (Simulated with
> the rdecent Master Branch of ngspice, adding 'set ngbehavior=ltpsa'
> to .spiceinit)

Thanks Holger, it work fine. With "TRAN 0.1u 5m", I get

Error: 449240 out of range for exp
...
doAnalyses: TRAN:  Timestep too small; time = 0.00177388, timestep =
1.25e-19: trouble with x1.x1:dx-instance d.x1.x1.d3
tran simulation(s) aborted

and the graphs are weird, but with "TRAN 5n 1m", all is fine.

From an old vacuum tubes radio, I made 3 of them for a theremin. One
with the FM triode for the volume and 2 with pentodes for the sound. I
get the first sounds yesterday, from infrasounds to ultrasounds. It is a
little weird to play but sounds already very good. For what I know, it
is the only theremin in existence with separated antennas.

-- 
If you have a problem and you are not doing anything to fix it, you are
at the heart of the problem.