LTspice simulation problem

meysaminter · May 23, 2012

Hi,
I want to simulate a power supply circuit in LTspice . but when I begin the simulation , it takes very long time and after two days it is steel simulating!!!!
during the simulating the " Damped Pseudo-Transient Analysis ...." fraze apear in software .I don't know my circuit has problem or my simulation progress ? simulating file and related library files for parts is attached . plz help me with this problem .

santhosh.vlsi · May 23, 2012

Hi..

Use the following in your design.

.options gmin=1e-10 abstol=1e-10 reltol=0.003

revart back if it works fine.............

Thank you

neddie · May 23, 2012

Change your simulation command to this :
.tran 10m startup

meysaminter · May 23, 2012

with "options gmin=1e-10 abstol=1e-10 reltol=0.003" following erorr apears :
.option syntax error, unrecognized option: "absol1e-10"
with ".tran 10m startup " the black area of resons apear but steel has an error :
Analysis: Time step too small; time=2.78385e-006, timestep=1.25e-019;trouble with u7:diode25-instance d:u7:_md1_d6

neddie · May 23, 2012

Go to the control panel. Under the spice tab , go to the "engine" area and choose "alternate" solver.
Not exactly sure what this does , but I'm sure the simulation results should still be valid. Any experts out there
can enlighten me if they choose :0)
There is also a yahoo group dedicated to LTSpice , can't remember the name but a search should turn it up quickly.

---------- Post added at 15:39 ---------- Previous post was at 15:26 ----------

Just noticed a few things on you diagram that arn't right. Your transformer has no coupling coefficients associated with it. k l2 l3 l4 1 will do for start.
R15 is 1 ohm , a little low I fear :0) Your resistive devider of R12 and R13 is going to give you an output higher than you would expect :0) R13 = 1ohm ,can't be right.
Also your transformer output is shorted between D5 anode and D1 anode.
Lucky for you this is a sim , else you may have some smoke wafting around :0)
Cheers
Ned

meysaminter · May 24, 2012

I corrected the transformer output but the feedback devider resistors are correct . I need 2.5 volt for Tl431 refrence . the output voltage of circuit must be 1000 volt and it seems to be true .
I have some problems now:
simulation continues to 2.7us and then "Analysis: Time step too small; time=2.78385e-006, timestep=1.25e-019;trouble with u7:diode25-instance d:u7:_md1_d6" erorr message is appear . I changed the "normal" to "alternate" in control panel the " Damped Pseudo-Transient Analysis ...." message appear again .Is this massege related to mistakes in Structure of circuit?
I guess there is a problem with IR2110. is IR2110 Properly connected to transistors?

neddie · May 24, 2012

Hi there.
Before going any further , calculate the power dissapation in your voltage divider resistors , that feed the TL431. The ratio may well be correct ( actually you are out by 10 times) , but I think you may want to revisit the values :0)

meysaminter · May 25, 2012

ok , I corrected the bottom resistor from 1 to 10 .

neddie · May 25, 2012

You still have not calculated the power dissipation in the resistors. With 1000Volts at the output , you are now going to need a 2.5W 1 ohm and a 2493W 399 ohm resistor.
Good luck finding the second one :0)
You need to increase the values significantly. 10K and 3.9Meg will get you close. The 3.9Meg would be better made of quite a few 100's of k resistors in series.

meysaminter · May 25, 2012

thanks neddie, you were right . so I changed the values to 10k and 3.99Meg .

meysaminter · May 25, 2012

but steel has "Analysis: Time step too small;..." error

---------- Post added at 10:44 ---------- Previous post was at 10:40 ----------

ok with changing"normal" to " Alternate" simulation is working and it is no error!!! but I want to have 1000 volt output and now it is 0 V!!!! can you help me with this?

neddie · May 25, 2012

Your cct is a bit of a mess. I've cleaned it up a bit and will attach. I've changed your FET's to more appropriate ones. Yours were only 20V devices , but you were using a 50V supply to your
bridge. Your feedback was not correct. You also had a 1ohm resistor pullup in the opto. It would never have been able to run correctly with such a low value pullup.
I've changed your feedback configuration and compensation. The turns ratio on the transformer is wrong. The voltage ratio is 1000/50 = 20 , so the inductance ratio is 400.
The inductance ratio is the square of the turns ratio. I've changed the Primary inductance to 20uH and the secondaries can be about 8mH give or take.
The driver chips were missing a connection to the bridge. There is a connection between the source of the high fet and the vs pin of the driver chip. One for each chip.It's part of the bootstrap cct that generates the high voltage for the top fet to switch.You had 1 ohm resistors in the source of each fet , not needed. I've changed a few other things , but you can check it out. Seems to be running ok , but I'd be careful if you are planning to actually build this :0)

Cheers
Ned

KerimF · May 25, 2012

When my simulation takes a relatively long time or doesn't converge, it is a sign for me that my circuit has one or more mistakes I missed to notice. Finding and correcting them, one after another, has its own joy

meysaminter · May 26, 2012

neddie, thank you very much .now simulation results 1000V output .and it is so cool!!! I have some qestion about the changes you madein circuit and I will ask you man.

---------- Post added at 08:52 ---------- Previous post was at 07:32 ----------

is output and input isolated? the GND of both sides seems to be same

neddie · May 28, 2012

They are isolated , via the transformer and the opto , but LTSpice only has one ground symbol/connection available. In practice they would be different grounds.
BYW , I've made a mistake with the feedback / compensation component connections. While it seems to work , it's not correct. I don't have much time at the moment , but
do some searching on the net to get some ideas of the correct connections. Just treat the error amp in the TL494 like any other opamp cct. When I get a chance ' I'll repost a better schematic.

neddie · May 29, 2012

This is a little better. Your TL431 model does not appear to be working very well. I'll attach another model.
I've added a little load to the system. (About 500W :0) ) , switches in after about 3mS. Changed the value of your output choke as well.
This in far from a perfect design , but will get you going. Someone with more SMPS design experience can chip in here and
get you further :0)

meysaminter · Jun 24, 2012

I am working on a new project and I need uc3854 LTspice model. Does anyone have it?

KerimF · Jun 25, 2012

meysaminter said:
I am working on a new project and I need uc3854 LTspice model. Does anyone have it?

Hi,

The attached files (in UC3844A.zip) are from:

**broken link removed**

Kerim

meysaminter · Jun 25, 2012

UC3854 not UC3844!!!!!!!!!!!!!!!!!!!!!

ZekeR · Jun 25, 2012

LTC is pretty good about building simulator models of their products into LTspice; however, they're usually not so good about building models of their competitors' parts. If you end up not being able to find one, or if you end up not being able to build one, you might be able to find a model built for TI's TINA simulator.

-Update-
TI provides a list of all the parts they've modeled here:
**broken link removed**
It seems the UC3854 isn't one of them.

LTspice simulation problem

Banned

Attachments

Newbie level 5

Full Member level 5

Banned

Full Member level 5

Banned

Attachments

Full Member level 5

Banned

Attachments

Full Member level 5

Banned

Attachments

Banned

Full Member level 5

Attachments

Advanced Member level 5

Banned

Full Member level 5

Full Member level 5

Attachments

Banned

Advanced Member level 5

Attachments

Banned

Full Member level 5

Similar threads

Privacy & Transparency

Privacy & Transparency