spice model for UL output transformer?
 User Name Stay logged in? Password
 Home Forums Rules Articles diyAudio Store Blogs Gallery Wiki 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
docali
diyAudio Member

Join Date: Oct 2004
spice model for UL output transformer?

Hi,

i would like to model an UL output XFMR and tried the following model but it yields an unsymmetric waveform. Do you have any hints how to do this?
Attached Images
 xfmr_ul.gif (7.1 KB, 2589 views)

 28th November 2005, 10:36 PM #2 Johan Potgieter   diyAudio Member   Join Date: May 2005 Location: Pretoria, South Africa Hi Docali, I have never used this, but the model looks over-simplified to me. There should also be resistance and capacitance somewhere, which parameters would certainly make a difference. Especially the latter; contrary to some perceptions the intersection capacitance is often the parameter limiting high frequency response, not the leakage reactance. Leakage reactance between primary sections need also be included; in fact any nearly accurate model would be quite complex i.m.o. The values would of course differ from unit to unit and C is mostly not given by manufacturers, thus I have chickened out in the past and settled for final response as measured in a real built-up unit. It would thus interest me as well and I hope someone with experience would broaden our horizons here.
 29th November 2005, 01:25 AM #3 Geek diyAudio Member     Join Date: Sep 2004 Here's a 3f4 spice model for a CT transformer from Circuit Maker: Code: ```*XTRANSCT:Transformer Subcircuit Parameters *XTRANSCT:RATIO:|Turns ratio= Secondary/Primary [1m,]|1 *XTRANSCT:RP:|Primary DC resistance [0,]|0.1 *XTRANSCT:RS:|Secondary DC resistance[0,]|0.1 *XTRANSCT:LEAK:|Leakage inductance[0,]|1u *XTRANSCT:MAG:|Magnetizing inductance[0,]|1u *{RATIO=1 RP=0.1 RS=0.1 LEAK=1u MAG=1u} *Generic ct secondary type:transformer .SUBCKT XTRANSCT 1 2 3 4 5 RPRI 1 7 {RP} LLEAK 7 10 {LEAK} LMAGNET 6 10 {MAG} VSEC1 9 4 DC 0V FSEC1 6 2 VSEC1 {(RATIO/2)} ESEC1 8 9 10 2 {(RATIO/2)} RSEC1 8 3 {(RS/2)} VSEC2 12 5 DC 0V FSEC2 6 2 VSEC2 {(RATIO/2)} ESEC2 11 12 10 2 {(RATIO/2)} RSEC2 11 4 {(RS/2)} .ENDS XTRANSCT *alias:XTRANSCT {RATIO=1} .PARAM A1TO1CT *alias:XTRANSCT {RATIO=.5} .PARAM A2TO1CT *alias:XTRANSCT {RATIO=.2} .PARAM A5TO1CT *alias:XTRANSCT {RATIO=.1} .PARAM A10TO1CT *alias:XTRANSCT {RATIO=.05} .PARAM A20TO1CT *alias:XTRANSCT {RATIO=.04} .PARAM A25TO1CT *alias:XTRANSCT {RATIO=.03448} .PARAM A29TO1CT``` I've found this model works great with resistances specified, rather than ratios. In your netlist, just edit as follows (for 5K primary, 40% UL example): Secondary: 0.08 (for 8 ohms) Primary plate to CT: 4 CT to V+: 1 Adjust other params as per transformer specs.
 29th November 2005, 07:02 AM #4 docali   diyAudio Member     Join Date: Oct 2004 Hi, thanks so far. I use LTSpice for simulations and it unfortunately does not work with 3f4 models. LTSpice only has a model for inductances but this model is good in my opinion, because it has model parameters for series resitance and capacitance. To model an UL transformer it should be possible to use two inductances in series with mutual inductance. The spice directive for this is for example: K1 L1 L2 0.999 But this did not work well in my simulations. Best regards from germany!
 29th November 2005, 09:19 AM #5 billr   diyAudio Member   Join Date: Dec 2003 Location: new zealand Have a look at this, it might help you, to get the UL windings, splt the primary using additional inductors, using the ratios that you need, link them, using mutual inductance, I have tried the non ul models Duncan provides and they seem to be ok. http://www.duncanamps.com/spicetransformers.html
 6th January 2006, 02:43 PM #6 jackinnj   diyAudio Member     Join Date: Apr 2002 Location: Llanddewi Brefi, NJ You can use a current-controlled current-source (or voltage controlled current sourc) and add the parasitic capacitance between primary and secondary add the leakage inductances and resistances on both sides of the device. Only problem with this approach is that it works down to DC. There are some good discussions on the theoretics of modeling non-linear RF transformers, transformers for switching supplies on the web, you just have to look.
Robert McLean
diyAudio Member

Join Date: May 2005
transformer spice models

Here are just two examples of how I do output transformers. They should work with any Spice variant as far as I know, I personally use LTSpice. I do have a vague recollection however that some spices wont allow more than 2 inductances on a K statement, so you have to put a seperate line for each pair of inductances.

Complex example, ie PP, UL, and multiple output taps.

.SUBCKT 1650R P1 Sg1 B Sg2 P2 O16 O8 O4 Com
* Push Pull transformer, with Ultralinear taps at 40%
* 5000 to 16 ohms, with 8 ohm and 4 ohm taps, 3db 15 to 60Khz
* Hammond 1650R
*
LP1 1 2 2.409088925H ; PRIMARY
LS1 2 B 1.070706189H ; primary, scrren grid tap portion
LS2 B 3 1.070706189H
LP2 3 4 2.409088925H
LA1 5 6 0.007348166H ; SPEAKER SECONDARY
LA2 6 7 0.003674083H
LA3 7 Com 0.021414124H
KALL LP1 LS1 LS2 LP2 LA1 LA2 LA3 0.999199994;
RP1 P1 1 30.0
RP2 Sg1 2 15.0
RP3 Sg2 3 15.0
RP4 P2 4 30.0
RS1 O16 5 0.1
RS2 O8 6 0.1
RS3 O4 7 0.1
.ENDS 1650R

P1 and P2 are the plate connections, B is the B+ connection, Sg1 and Sg2 screen grid connections, and O16, O8 and O4 the 16, 8 and 4 ohm outputs, and Com the common secondary terminal

Simplest example, ie SE, single output.

.SUBCKT 5KSE P1 P2 Sp1 Sp2
* Single ended audio transformer
* 5k to 8 ohm, 10 to 40KHz
*
LP1 1 P2 40.26021568H ; PRIMARY
LSA 2 Sp2 0.064416345H ; SPEAKER SECONDARY
KALL LP1 LSA 0.999499875 ;
RP1 P1 1 56
RS Sp1 2 .1
.ENDS

P1 and P2 are the primary ie plate connections, and Sp1 and Sp2 the secondary ie speaker connections.

When loaded by the specified input and output resistances they give the specified frequency response. They include winding resistance so you get the expected voltage drops. These are purely linear models and so do not give any distortion. So they are not realistic in that regard, but the fact that the taps "work right", ie the ultralinear acts as it should, and you can put 4 ohms on the 4 ohm tap or 8 ohms on the 8 ohm tap and get the right results make them very useful in my opinion. The frequency response may not have all the little quirks of the real transformer, but it is reasonable, not DC to infinity or anything like that.

I use the attached spreadsheet to derive the model parameters. The values given for the various transformers listed are taken from various data sheets and websites and so on. Many of the dc resistances are just pure guesses on my part. I make no claim that the models will match the real transformer, only that the model will have the frequencey response and impedance ratio that the spec sheet claims for the real transformer.

The spreadsheet is just something I whipped up for myself, so it is not particularly user friendly perhaps, but it should be fairly easy to use. Just input nominal source impedance, output impedance, winding resistances and upper and lower 3dB frequencies, and then in the rightmost columns you will get KA, LP and LS for SE types, or KA, LP1, LP2, and LS2 for PP types. Paste those values into the spice model. If you want multiple output taps then take the value for LS and paste it into cell A7 on sheet 2, set the tap impedances as required ( default is 4, 8, and 16) and then see the values for LA1, LA2 and LA3. Paste these into the spice model.
Attached Files
 transformer model parameters.zip (16.8 KB, 1180 views)
__________________
Robert McLean

 8th August 2007, 02:18 PM #8 StoneT   diyAudio Member   Join Date: Jan 2007 Location: Devon UK Good work... Looks like alot of thought went into that, nice one. On a related note: I recently bought a bargain pair of hammond 1615 output transformers (which match your table reasonably well) but when I put the measured specs (LP, LS, DCRs...) into my LTpice simulation it didn't perform as well as expected. Normally these have a Zp-p of 5000 but I am using them with 8ohms on the 4ohm taps to get a Zp-p of 10000. I thought that this was the problem for a while and was quite disheartened as my design didn't seem able to produce a 50Hz square wave of more than about 2W without entering class B with the 1615. (It is supposed to be a 7 - 8W pure class A amp). However I now realise that it was the NFB that was the problem. As the output level falls on the tops of the square wave the amp tries to miantain the level through the transformer resulting in the drive signal to the output tubes increasing. As my NFB was quite substantial it tried to maintain the output exactly by a huge increase in drive signal resulting in one valve shutting off. Seems obvious now but it vexed me for quite some time. Just thought the info might be usefull for anyone else in the same situation. Incidentally- The differences between my measurements and your specs on the spreadsheet are mainly the primary DCR (You show 30 Ohm on each primary, I measured about 84 and 90), and the Lprimary (yours is about 6 in total, I measured about 2.4, which might account for the perfomance of your model being better at low frequencies than the hammond specs) __________________ StoneT
 8th August 2007, 03:33 PM #9 jackinnj   diyAudio Member     Join Date: Apr 2002 Location: Llanddewi Brefi, NJ A really good PDF on transformer modeling: http://www.eettaiwan.com/ARTICLES/20...A_DA_AN215.PDF Here's a Hammond 1608 with 8R on the secondary and 5k6 on the primary -- don't forget the interwinding capacitance in your model:

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is Off Forum Rules
 Forum Jump User Control Panel Private Messages Subscriptions Who's Online Search Forums Forums Home Site     Site Announcements     Forum Problems Amplifiers     Solid State     Pass Labs     Tubes / Valves     Chip Amps     Class D     Power Supplies     Headphone Systems Source & Line     Analogue Source     Analog Line Level     Digital Source     Digital Line Level     PC Based Loudspeakers     Multi-Way     Full Range     Subwoofers     Planars & Exotics Live Sound     PA Systems     Instruments and Amps Design & Build     Parts     Equipment & Tools     Construction Tips     Software Tools General Interest     Car Audio     diyAudio.com Articles     Music     Everything Else Member Areas     Introductions     The Lounge     Clubs & Events     In Memoriam The Moving Image Commercial Sector     Swap Meet     Group Buys     The diyAudio Store     Vendor Forums         Vendor's Bazaar         Sonic Craft         Apex Jr         Audio Sector         Acoustic Fun         Chipamp         DIY HiFi Supply         Elekit         Elektor         Mains Cables R Us         Parts Connexion         Planet 10 hifi         Quanghao Audio Design         Siliconray Online Electronics Store         Tubelab     Manufacturers         AKSA         Audio Poutine         Musicaltech         Holton Precision Audio         CSS         exaDevices         Feastrex         GedLee         Head 'n' HiFi - Walter         Heatsink USA         miniDSP         SITO Audio         Twin Audio         Twisted Pear         Wild Burro Audio

 Similar Threads Thread Thread Starter Forum Replies Last Post lcsaszar Software Tools 4 8th August 2008 02:02 PM porcatroya Tubes / Valves 0 5th May 2008 06:41 AM classd4sure Power Supplies 3 20th July 2006 03:50 PM Paracelsus Tubes / Valves 6 9th September 2005 02:52 PM Prune Software Tools 6 16th October 2004 03:22 PM

 New To Site? Need Help?

All times are GMT. The time now is 04:24 AM.