LTSpice PSU simulation help - SoftStart modeling

[ninjanki]

Hi,

I am new to writing to the forum, but I've been reading it for a while, and after a lot of tought, I decided that building an UCD based amplifier would be a nice DIY-project for my HT. Key trouble here is that I need to design the power source for that amplifier, and I got stuck at the softstart design.

I have read both the TNT and Zero-Distortion articles about power supply design, and I've got the transformer, retification and filtering worked out and being simulated on LTSpice. When I tried to add a softstart to this simulation, I noticed that LTSpice has some kind of trouble with controled-switches(CSW and VSW), which would be the equivalent of real-life relays. I could not find models on the internet that actually worked on LTSpice, and so I am unable to proceed on that front...
Does anyone has experience with LTSpice modeling, and could help me with it? If not, does someone have a schematic for a complete softstar circuit that could be added to a 600VA PSU?

Thanks,
Allan

 

[peranders]

Soft start isn't so complicated. We have covered this before. Just check here:

http://www.diyaudio.com/forums/showthread.php?s=&threadid=23540&highlight=
http://www.diyaudio.com/forums/showthread.php?s=&threadid=6236&highlight=
http://www.diyaudio.com/forums/showthread.php?s=&threadid=44886&perpage=20&highlight=&pagenumber=1
http://www.google.se/search?hl=sv&ie=ISO-8859-1&q=soft+start+toroids&btnG=Google-s%F6kning&meta=
http://www.google.se/search?hl=sv&ie=ISO-8859-1&q=soft+start&btnG=S%F6k&meta=

 

[ninjanki]

peranders,

I eventually found some of the examples you pointed out(before seeing your response). I guess I'll have to use one of the ready schemes and hope it is a working one....(since I still can't simulate using LTSpice - any clue about why it does not have a working switch model?)

On a secondary question I found latter, my simulations seem to indicate current peaks of about 140A on the rectifier diodes, during normal operation with about 30mF of filtering and a resistive 4 ohm load. Are these peaks ok for the diodes, right?(considering peak current can be much higher than nominal current, 35 amps)
What about the capacitors, can they handle those peaks? Or I do have something wrong with my capacitor data use on the modeling?

Thanks,
Allan

 

[ghemink]

peranders,

I eventually found some of the examples you pointed out(before seeing your response). I guess I'll have to use one of the ready schemes and hope it is a working one....(since I still can't simulate using LTSpice - any clue about why it does not have a working switch model?)

On a secondary question I found latter, my simulations seem to indicate current peaks of about 140A on the rectifier diodes, during normal operation with about 30mF of filtering and a resistive 4 ohm load. Are these peaks ok for the diodes, right?(considering peak current can be much higher than nominal current, 35 amps)
What about the capacitors, can they handle those peaks? Or I do have something wrong with my capacitor data use on the modeling?

Thanks,
Allan

That current will never occur in real life, try putting a small resistor in series with your power mains in the simulation, if you pull 140A out of your wall mains socket, I`m sure the voltage will drop quite a bit. I think I usually add about 1 ohm series resistance, the tranformer will have series resistance as well. Probably current peaks like 20-30 amps are more normal.

I could simulate the switch in LTspice. I used voltage controlled switches to make a simplified switch to simulate a UcD like amp.

Gertjan

 

[ninjanki]

Gertjan,

Thanks for the confirmation about what is the problem with my model. I was guessing that either I was missing some series resistance or some parameter on the capacitor definition(I noticed that capacitor inductance can affect these peaks by great amounts....)

About the switch simulation, maybe I am just missing some basic info. When I try to use a voltage controled switch, it tells me that there is no model defined for it. I am probably missing some information about how to use it. Could you write down a simple example of how to insert such a switch on LTSpice? What parameters, and where shoud I insert them?

Thanks,
Allan

ps. What can I use to simulate a toroid? I havent seen those on LTSpice either... Right now, I am working with both sides of the tranformer independently cause I can't find a transformer model... I am probalby just being lazy or blind...

 

[peranders]

That current will never occur in real life, try putting a small resistor in series with your power mains in the simulation, if you pull 140A out of your wall mains socket, I`m sure the voltage will drop quite a bit.

High currents _will occur. I have used a 75MHz hall-effect current probe and got 77A with 2 x 300 VA UNCONNECTED, no load!

 

[jcx]

for LTSwCAD spice questions there is a very useful, active, responsive group on Yahoo - you need to get free a yahoo membership to join though

many questions can be solved by looking through the example files included with LtSwCAD, more example files are at the Yahoo group

Try reading the really fine help file in Lt spice, there may be naming convention or device/subcircuit arg variations but nearly all standard spice examples I have tried work without modification

you can create a transformer sub circuit and symbol if you want but the spice primitive is to add a coupling coefficient statement "K" linking independently named simple inductors for each winding:

L1 1 2 100u
L2 3 4 400u
K1 L1 L2 0.99

 

[JonHarrison]

Allan,

I've been here myself when I was modelling a psu design.

Try this. Use the voltage controlled switch 'sw' in the main group. Set the SpiceModel for the switch to RELAYSW and then on your schematic add the following spice directive to define the model

.model RELAYSW SW(Ron=6 Roff=1G Vt=22 Vh=.4)

Ron is the on resistance of the 'relay' - 6ohms
Roff, the off resistance 1GIG ohm
Vt is the turn on voltage
Vh is the hysterisis

Cheers,

Jon

 

[ninjanki]

jcx,

Thanks for the quick explanation on transformers using LTSpice. After i got your lead, I was able to find documentation and understand how LTSpice handles it(i did not understand the use of the .op option until then...) Do you have any idea on the parameter I should use for the inductors? I am trying to build good models for two toroids, one of 625VA and another one of 800VA. After simulating for a while, these are the ones I got:

800VA - 127V -> (30V - 13A)x2

L1: 18H R:0.95 L2&L3: 1.46H R:0.27

800VA - 127V -> (40V - 10A)x2

L1: 18H R:0.84 L2&L3: 2.29H R:0.3

Since I do not have experience with transformers, and I could not find the inductance data on any datasheet, I am not sure if these values are in the balpark of the real thing or not...

Jon,

I used your example as a reference, and I have a switch working for my softstart circuit. Thanks'for the help!

Allan

 

[ninjanki]

A few corrections to the last post... The models I made, which probably have wrong inductance values compared with the real thing, are just for 800VA transformers, and the nominal voltage is 115V, not 127...

Allan

 

[jcx]

line power xfmrs have very nonlinear core operating point - the manufacturers don't make money by giving you more iron and Cu - you have to spec it and pay for it in a custom design

nonimal inducatnce can be determined from the primary current with the secondary open - Line V warning! don't mess around

sec inductance is proportional to pri L by n^2, R series is easily measured, line xfmr K usually a question of "how many 9s" - .99, .999, ...

inrush sim will be inaccurate due to core nonlinearity - core sat models can be done but are complicated - the nominal linear model at least gets you started but you'll have to measure the real thing