
Home  Forums  Rules  Articles  The diyAudio Store  Gallery  Blogs  Register  Donations  FAQ  Calendar  Search  Today's Posts  Mark Forums Read  Search 
Tubes / Valves All about our sweet vacuum tubes :) Threads about Musical Instrument Amps of all kinds should be in the Instruments & Amps forum 

Please consider donating to help us continue to serve you.
Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving 

Thread Tools  Search this Thread 
7th August 2008, 04:13 PM  #1 
diyAudio Member
Join Date: Mar 2004
Location: Budapest, Hungary

PSpice model of output transformer
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/Tub...e_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 
8th August 2008, 05:10 AM  #2 
diyAudio Member
Join Date: Mar 2008

I couldn't find your schematic.

8th August 2008, 10:41 AM  #3 
diyAudio Member
Join Date: Mar 2004
Location: Budapest, Hungary

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.

8th August 2008, 02:17 PM  #4 
diyAudio Member

Here's the Multisim audio transformer model
.SUBCKT ts_audio_ideal 1 2 3 4 5 * EWB Version 4  Transformer Model * n= 2 Le= 1e006 Lm= 0.001 Rp= 1e006 Rs= 1e006 Rp 1 6 1e006ohm Rs1 10 3 1e006ohm Rs2 11 5 5e007ohm Le 6 7 1e006H 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 1.000e3 Rl2 31 3 1.000e3 Rl3 41 4 1.000e3 L1 11 2 5.000e+000 L2 31 5 5.000e002 L3 5 41 5.000e002 K12 L1 L2 9.999e001 K13 L1 L3 9.999e001 K23 L2 L3 9.999e001 .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. 
8th August 2008, 03:02 PM  #5 
diyAudio Member
Join Date: Mar 2004
Location: Budapest, Hungary

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} ; QFACTOR. 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} ; 816 OHM WINDING: (2SQRT(2))^2 LP6 8 7 {.17157*LPRIM*LRATIO} ; 48 OHM WINDING: (SQRT(2)1)^2 LP7 9 8 {LPRIM*LRATIO} ; COM4 OHM WINDING KALL LP1 LP2 LP3 LP4 LP5 LP6 LP7 {11/(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 
Thread Tools  Search this Thread 


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
spice model for UL output transformer?  docali  Tubes / Valves  30  5th May 2013 01:52 AM 
New 12AX7A Pspice model  eppidei  Tubes / Valves  17  20th January 2008 07:01 AM 
I need 2SC2570 PSPICE Model  xitronics  Parts  1  10th July 2006 09:29 AM 
HIP4080A pspice model  Anthony C Smith  Class D  1  3rd January 2006 08:52 PM 
output transformer spice model  Paracelsus  Tubes / Valves  6  9th September 2005 03:52 PM 
New To Site?  Need Help? 