#49 JFET DC TEMP SIMULATION PROBLEM

[SERGEY CHURAYEV]

Hi all,

I got 2 different simulation problem in JFET DC TEMP SIMULATION.
1st picture is results from LTSPICE, another one from Ngspice.
I know what the 1-st is OK.
Tell me please, is it something wrong with Ngspice or my code?

LTSPICE code:
VD 1 0 DC 10V
VDMI 1 3 0
VG 2 0 DC 0V

---

• D G S *

---

J1 3 2 0 KP303D

.model KP303D NJF (Beta=1.5m Betatce=-.5 Rd=1 Rs=1 Lambda=4.2m Vto=-2.3

• Vtotc=-2.5m Is=33.57f Isr=322.4f N=1 Nr=2 Xti=3 Alpha=311.7u
• Vk=243.6 Cgd=2.132p M=.3622 Pb=1 Fc=.5 Cgs=2.104p Kf=23.06E-18 Af=1)

.TEMP -60 0 27 125 ;

.DC VG -2.5V 3.5V 0.1V ;

.PROBE ID(J1)

.END

NGSpice code:

VD 1 0 DC 10V
VDMI 1 3 0
VG 2 0 DC 0V

---

• D G S *

---

J1 3 2 0 KP303D level2

.model KP303D NJF (Beta=1.5m Betatce=-.5 Rd=1 Rs=1 Lambda=4.2m Vto=-2.3

• Vtotc=-2.5m Is=33.57f Isr=322.4f N=1 Nr=2 Xti=3 Alpha=311.7u
• Vk=243.6 Cgd=2.132p M=.3622 Pb=1 Fc=.5 Cgs=2.104p Kf=23.06E-18 Af=1)

.control
set xbrushwidth=3
foreach tvar -60 0 60 120
set temp = $tvar
DC VG -2.5V 3.5V 0.01V
run
end
plot all.VDMI#branch
.endc

.END

Thank you.

[Dietmar Warning]

Sergey,
your code is right at most. Only the instance parameter "level=2" is wrong but will be omitted.
The problem is, that both simulators have different temperature models for jfets implemented. You see the warnings about ignored parameters in the ngspice console.
Please try this modified model card in ngspice:
.model KP303D NJF (Beta=4m

• bex=-1.2
• Rd=1 Rs=1 Lambda=4.2m Vto=-2.3
• tcv=1m
• Is=33.57f
• Cgd=2.132p M=.3622 Pb=1 Fc=.5 Cgs=2.104p Kf=23.06E-18 Af=1)
  It is a first trial of hand tuning the parameters Beta, bex, and tcv.
  The temperature model in LTspice is not published so far I know.
  Good luck,
  Dietmar

[SERGEY CHURAYEV]

Dear Dietmar,

Thank you!
You are right, now it work.

Tell me please about + M=.3622
It looks like this coefficient does not exist in current specification.
But it exists in Pspice mod. And I did not see any warning in NGSPICE log.
Without it simulation works more realistic (as I see).

===============================

VD 1 0 DC 10V
VDMI 1 3 0
VG 2 0 DC 0V
J1 3 2 0 KP303D

.model KP303D NJF

• (
• Vto=-2.3
• Beta=1.5m
• Lambda=4.2m
• Rd=1
• Rs=1
• Cgs=2.104p
• Cgd=2.132p
• Pb=1
• Is=33.57f
• B=1.1
• Kf=23.06E-18
• Af=1
• NLEV=1
• GDSNOI=1.0
• Fc=.5
• TNOM=27
• tcv=1m
• bex=-0.5
• )

.control
set xbrushwidth=2
foreach tvar -60 -30 0 30 60 120
set temp = $tvar
DC VG -2.5V 0.5V 0.01V
run
end
plot all.VDMI#branch
.endc

.END

==========================================

[Dietmar Warning]

Hi Sergey,
I aggree with the seamless acception of model parameter "M" seems something wrong. For LTspice is it the grading coefficient of the gate junction. Same as for temperature model in ngspice was another equation used.
But not to issue a warning is a bug. Seems something in the netlist interface gone wrong. Perhaps Holger can help. The model parameter "m" arrived not the model interface routine jfetmpar.c.
It should possible to implement some of the Pspice extensions into our jfet model so far we can find the equations.
Thank you,
Dietmar

[Holger Vogt]

In our models 'm' is the parallel multiplier.

In PSPICE 'm' is the 'gate p-n grading coefficient'.
In our model we have something like 'b' which is the 'Doping tail parameter'.
I have not checked how these two relate to each other.

The PSPICE JFET equations are shown in the PSpice Reference Guide.

[SERGEY CHURAYEV]

Dear all.
Thanks for your details explanation.
I got very realistic results and we can close this ticket.
I will inform you if I will get more issues in NGspice.
Good luck!

[Dietmar Warning]

alternative temperature model for certain jfet parameter is implemented in pre-master branch