Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

UC3842 model is not working at all

Greetings, I am trying to simulate switching regulator circuits with Multisim 10.

 

Specifically, I am trying to use the UC3844 model to create a boost regulator, buck regulator, and eventually a flyback regulator.

 

The UC3844 part is pretty easy to work with in real life, but is not functional in Multisim10.

 

The datasheet is from texas instruments -- SLUS223C

 

Try the example circuit on Page 7 from SLUS223C in Multisim.

 

I noticed that the Vref pin never has 5Vdc present during the simulation.  In real life, there is always 5Vdc present on the Vref pin as soon as the DC voltage on VCC rises above 16Vdc.

 

It's as though the part is not turning on or is stuck in undervoltage lockout.

 

Can anyone explain how this part is supposed to work in multisim 10, or is there a working example multisim simulation example I can reference?

0 Kudos
Message 1 of 7
(15,038 Views)

Could it be possible that are using a component that does not have a simulation model attached to it?

 

I quickly tested the UC3842 component, and correctly saw 5V on the reference pin.  But the variants of this component (ie. the UC3842A_DIP8, UC3842_SO8 etc.), are for schematic capture/layout only and have no simulation models linked to them.  If this is the case, try swapping the component for the UC3842.

 

If you're still having trouble, post your circuit; it's always easier to pinpoint the issue that way!


Natasha Baker
R&D Engineer
National Instruments

Join the NI Circuit Design Community
Follow Multisim on Twitter!
0 Kudos
Message 2 of 7
(15,034 Views)

Hello Natasha,

 

I checked and you are exactly right, the model information is not present in ANY of the UC384x parts.  Apparently none of the UC3844_ parts in my library have models. 

 

How can I get the model info to fix this?

 

Thank you!

0 Kudos
Message 3 of 7
(15,030 Views)

There is a base part with simulation model, which is just UC3842 located in the Analog, SPECIAL_FUNCTION family.  (The only version of Multisim that does not have access to this component is the Student version.)


Natasha Baker
R&D Engineer
National Instruments

Join the NI Circuit Design Community
Follow Multisim on Twitter!
0 Kudos
Message 4 of 7
(15,023 Views)

Negative Natasha, all I find in analog( special function) is INA126P, PA, U, UA, nothing else.

I'm using Multisim 10.1 power pro edition.

 

Curiously, when I search for UC3842 - Group-ALL, Family-ALL I get something, when click ok, INA126P appears in nice blue color(Model included) ready to be placed.

 

Thank you for your help. 

0 Kudos
Message 5 of 7
(14,661 Views)

kiki_barrios,

 

Hello - attached is the UC3842 model you are looking for in v10.1 in a flyback topology (modified from existing SMPS samples).   I suggest that for Switch Mode Power Controllers that you also reference the SMPS samples (File -> Open Samples -> SMPS).   Many of sample circuits in the topologies shown have corresponding SMPS controller ICs models with parametric values that allow you to match the specifications closely with the manufacturer's IC specifications.  The sample I included swapped out the BASSO model for the UC3842 model.

 

Recently a customer looking for a Linear Technologies SMPS controller (not in the DB) was successfully able to use a corresponding PWMCM BASSO model in lieu of the actual mfg SPICE model as many of these are propietary or encrypted.  

 

These BASSO models are relatively easy to use.  For a given topology (CM or VM, buck, boost, flyback), open up the sample circuit.  Adjust the model by opening up the SPICE model of the controller within the circuit (Double-click on part -> Edit Model button).   Adjust the 'Current Instance Parameters:' to match those found on the datasheet as shown below.  

 

PWMCM model.JPG

 

Multisim customers that are using these, say there is close agreement to the simulations compared to what they see on the benchtop during verification testing.

 

Also in general I find when using these SMPS samples in your own applications, adjusting the simustion engine parameters 'RSHUNT' a few decades down (from default of 10^12 -> 10^11 or 10^10) [due to high C, L values] and adjusting the integration method 'METHOD' from 'trapezoidal' to 'gear' [due to switching signals] allows for better convergence performance of these models and SMPS circuits in general.   These settings are found in the Multisim menu as follows: (Simulate -> Interactive Simulation Settings -> Analysis Options [tab]-> Select 'Use custom settings' (hit 'Customize' button) -> locate/change the corresponding engine paramenters as indicated above).

 

By the way,  Basso's 'Switch-Mode Power Supply SPICE Cookbook ' is also a good reference for your design requirements as the examples in this Multisim sample folder are based on this book.

 

Hope this helps.

 

Regards,

Patrick Noonan

National Instruments

Message 6 of 7
(14,639 Views)

User32

 

Hello,

 

Thank you for your prompt response, you solved my problem and taught me a lot at the same time.

Excellent job, very impressive.

 

Thank you very, very much.

 

 

 

0 Kudos
Message 7 of 7
(14,619 Views)