Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

LTspice simulation problem

Status
Not open for further replies.
meysaminter

meysaminter

Banned
Member level 3
Joined
Dec 19, 2009
Messages
59
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,296
Visit site
Activity points
0
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 .
 

Attachments

  • LTspice simulation.zip
    3.8 KB · Views: 294
  • Lib files.zip
    19.7 KB · Views: 234

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
 

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
 

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
 
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?
 

Attachments

  • simulation.zip
    4 KB · Views: 185
Last edited:

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

Attachments

  • LTspice simulation.rar
    3.6 KB · Views: 267
Last edited:

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

Attachments

  • LT.zip
    3.8 KB · Views: 192

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?
 

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
 

Attachments

  • Draft2.zip
    2.4 KB · Views: 179
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 ;)
 
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
 
Last edited:

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.
 

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)
 

Attachments

  • tl431.zip
    1.2 KB · Views: 195
  • 1000V power supply V2.zip
    2.6 KB · Views: 189
I am working on a new project and I need uc3854 LTspice model. Does anyone have it?
 

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.
 
Last edited:

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top