PSpice model of output transformer

[lcsaszar]

Hi all,

I am new in this field, and I want to use PSpice for modelling audio circuits (mostly tube circuits). I downloaded the tube.lib from Norman L. Koren's site:

http://www.normankoren.com/Audio/Tubemodspice_article.html

I am really stuck in creating a model of output transformer. It should be quite simple, a primary with a center tap, a secondary with a center tap. It can be characterized by the turns ratio in the first run. (Its model can be modified later by including primary and secondary inductance, coupling coefficient or stray inductance, and primary and secondary resistance, and later perhaps self and mutual capacitances). Do you know of any good SPICE model of such transformer?

I attached my schematics (a working amplifier of my design, that I want to optimize with SPICE). The problem is when I run simulation, it gives an error which is most probably related to the output transformer. I tried to edit the OUTPUT_XFRMR symbol, but no avail. Could someone please have a look at my schematics, and help me find what is the problem? Please forgive me if it is a very stupid problem, but as I said, I am an absolute beginner.

Thanks in advance,

Laszlo

 

[exeric]

I couldn't find your schematic.

 

[lcsaszar]

Here is my schematics. I replaced OUTPUT_XFRMR with DYNA_OUTPUT_XFRMR. Now it does work, I just have to figure out how to do AC and Fourier analysis.

 

[jackinnj]

Here's the Multisim audio transformer model

.SUBCKT ts_audio_ideal 1 2 3 4 5
* EWB Version 4 - Transformer Model
* n= 2 Le= 1e-006 Lm= 0.001 Rp= 1e-006 Rs= 1e-006
Rp 1 6 1e-006ohm
Rs1 10 3 1e-006ohm
Rs2 11 5 5e-007ohm
Le 6 7 1e-006H
Lm 7 2 0.001H
E1 9 8 7 2 0.25
E2 8 4 7 2 0.25
V1 9 10 DC 0V
V2 8 11 DC 0V
F1 7 2 V1 0.5
F2 7 2 V2 0.5
.ENDS

Here's a model for a power transformer using K coupling factors:

.SUBCKT ts_pwr_10_to_1 1 2 3 4 5
* *1, 2-- primary winding, *3,4-- secondary terminal, 5-- neutural
Rs1 1 11 1.000e-3
Rl2 31 3 1.000e-3
Rl3 41 4 1.000e-3
L1 11 2 5.000e+000
L2 31 5 5.000e-002
L3 5 41 5.000e-002
K12 L1 L2 9.999e-001
K13 L1 L3 9.999e-001
K23 L2 L3 9.999e-001
.ENDS

For a center tap use the transformer backwards and adjust the inductance to reflect the primary and secondary impedances.

You might find the 2nd set easier to use -- if you are modeling a real world transformer you would probably put in interwinding coupling capacitance between nodes 11 and 31 of a few hundred pF's, and some additional inductance on the primary and secondary.

 

[lcsaszar]

Thanks, I can at least start with this. Also the DYNA_OUTPUT_XFRMR does work, I just need to adjust the parameters of the transformer.

----------------------------------------
.SUBCKT DYNA_OUTPUT_XFRMR 1 2 3 4 5 6 7 8 9 ; PARAMETERS FOR MARK 3:
+PARAMS: LPRIM=60 LLKG=.040 RPRIM=125 CPRIM=1.04NF LRATIO={4/4300}

* ERIC BARBOUR ARTICLE: ~233H TOTAL PRIMARY L FOR MARK 3.
* MARK 3: LPRIM=60 LLKG=.040 RPRIM=125 CPRIM=1.04NF LRATIO={4/4300}

* LPRIM IS THE TOTAL PRIMARY L (VARIES WITH MEASUREMENT).
* LLKG IS THE LEAKAGE L (MEASURABLE: CONSISTENT).
* RPRIM IS THE TOTAL PRIMARY R.
* CPRIM IS THE MEASURED PRIMARY CAPACITANCE.
* LRATIO IS THE INDUCTANCE RATIO: (4 OHMS)/(PRIMARY Z).

.PARAM QFCTR={LPRIM/LLKG} ; Q-FACTOR.
CS1 1 5 {CPRIM} ; PRIMARY CAPACITANCE
RS1 1 5 300K ; SHUNT R FOR HIGH FREQUENCY EFFECTS.
LP1 1 12 {LPRIM*.09} ; .7164H ; PRIMARY
RP1 12 2 {RPRIM*.5}
LP2 2 3 {LPRIM*.04} ; .3184H
LP3 3 4 {LPRIM*.04}
LP4 4 45 {LPRIM*.09}
RP4 45 5 {RPRIM*.5}
LP5 7 6 {.34315*LPRIM*LRATIO} ; 8-16 OHM WINDING: (2-SQRT(2))^2
LP6 8 7 {.17157*LPRIM*LRATIO} ; 4-8 OHM WINDING: (SQRT(2)-1)^2
LP7 9 8 {LPRIM*LRATIO} ; COM-4 OHM WINDING
KALL LP1 LP2 LP3 LP4 LP5 LP6 LP7 {1-1/(2*QFCTR)} ; COUPLING
.ENDS
----------------------------------------

My other problem is that I can not find the diode.slb library. I found diode.lib and diode.olb, but I can not convert them to diode.slb whatever I do. Any advice would be appreciated