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.

Pspice, UC3845 & Boost Converter

Status
Not open for further replies.

irshad

Newbie level 4
Joined
Jan 27, 2006
Messages
6
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,332
boost converter pspice

hi, i'm new here & would like to single phase develop boost converter by using uc3845 with pspice (which is the part in the library). i try to do simulation but error occur. plz help me to get the best reference in Pspice. TQ
 

v_c

Advanced Member level 2
Joined
Oct 11, 2005
Messages
514
Helped
113
Reputation
226
Reaction score
37
Trophy points
1,308
Location
Chicago, IL, USA
Activity points
8,229
boost converter spice

Well, what kind of errors are you getting? You have to be specific with your problems and give some additional information (operating condition, other specifications) to get a useful answer. If you present a vague problem, you will get vague (and useless) answers and followups that ask for additional information.

I assume that you already have the datasheet from Texas Instruments (or Fairchild) that is given here AC/DC and DC/DC Power Supplies - PWM Power Supply Controllers - UC3845 - TI.com
Look in the back of the document on page 7 for a circuit based on the flyback topology.

There is document here on understanding the boost power stage https://focus.ti.com/lit/an/slva061/slva061.pdf
Make sure that you understand this document. Before actually applying the controller into your system, you have to make sure that your topology can run in open-loop -- just drive your MOSFET with a volage pulse of a given frequency and duty ratio and make sure that the voltage ripple, current ripple, etc. are satisfied.

Best regards,
\[v_c\]

Added after 22 minutes:

Also take a look at Texas Instruments Reference Designs Power Management Single Output Reference Designs
These are design examples that feature a particular type of controller IC.
There is nothing for the 3845 but any generic PWM controller of same type should give you an idea.

It might give you some ideas if your design is still open. If you already have your design and simulation is your only issue -- then please post the specific errors. I am quite certain I can help you out.

Best regards,
v_c
 
Last edited by a moderator:

irshad

Newbie level 4
Joined
Jan 27, 2006
Messages
6
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,332
uc3845 spice

Thank you for your info. it's really helpful.

I tried to built the charge pump circuits (which i got from Unitrode application note) but the errors occur as following:
1) In session log: "No PSpice Templete for U3 (refer to the IC), ignoring''
2) Prompt msg: The string 'Error" was not found
3)In Pspice A/D:
Error-- less than 2 connections at node N04935
Error-- Node N04950 is floating
Error-- Node N04935 is floating (This node connected to Vref of IC)

For your information i get the uc3845 ic from Orcad/Capture/Library/regulator.olb.
 

v_c

Advanced Member level 2
Joined
Oct 11, 2005
Messages
514
Helped
113
Reputation
226
Reaction score
37
Trophy points
1,308
Location
Chicago, IL, USA
Activity points
8,229
uc3845 pspice

error 1 is saying that you don't have a pspice model (not the symbol but the spice subcircuit) that corresponds to U3. Check to make sure that you actually have a library that has this subcircuit. The libraries are ASCII files that you can open with a text editor. And the model should be between lines ".subckt" and ".ends" statements.

error 3 regarding the floating nodes happens quite often if the node in question does not have a dc path to ground -- this results in a singular matrix and spice cannot solve the system. The easy remedy for this is to put large value resistors like 10Meg from those nodes down to ground and make sure the circuit is not affected by the change. What is happening in these situations is that at the initial dc solution capacitors are open circuits and inductors are short circuits. And in this situation, you probably have some nodes in your circuit that do not have a path to ground. This is what you have to fix. error 3 is happening because we are assuming that a capacitor, for example, is ideal. But in reality, it really has parasitic resistances and inductance associated with it. So when you build the actual circuit, you will not have such "floating nodes".

Best regards,
v_c

If you can post your netlist, I might be able to help further.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top