Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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 Simulation of a Boost Converter

Status
Not open for further replies.

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
pspice schematic+boost converter

Does anybody know how i can vary the voltage source in the middle of a transient analysis ? i want to observe the variation of the output voltage due to the changing of input voltage in the middle of a transient analysis. thank you very much.
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost converter pspice

Changing the voltage at required time in the stimulus of the input voltage source in question is not ok?

Best Regards
Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
vpwl pspice

hmnn ... you just gave me an idea ... by using stimulus.. thank you thank you but do you mean changing the vsource to a stimulus ? and if so ... which stimulus should i use ? in my source library, there are a few stimulus... unsure which one to use though ... thank you.
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
pspice simulation boost

What type of voltage source are you using? (Is it a constant voltage source?)

Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

Nimer

Full Member level 3
Joined
Apr 26, 2005
Messages
180
Helped
26
Reputation
52
Reaction score
8
Trophy points
1,298
Location
PALISTINE
Activity points
2,907
boost pspice simulation

high
if you are using dc source youcould use the dc sweep analysis to vary the the source in arange of values

best regards
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost pspice schematic

Nimer said:
...if you are using dc source youcould use the dc sweep analysis to vary the the source in arange of values...

but mengghee wants to change the voltage during a transient analysis...

In my opinion there is no problem to use, say, a VPWL source (piecewise linear voltage source) and define required time flow of the input voltage.

Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
boost converter using pspice

Eric, I am just using a normal voltage source in my souce library 'VDC'. and what is 'VPWL' ???. nimer, i cannot use DC sweep because i need the transient analysis.
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost orcad capture converter

mengghee said:
Eric, I am just using a normal voltage source in my souce library 'VDC'. and what is 'VPWL' ???. nimer, i cannot use DC sweep because i need the transient analysis.

mengghee, if you use PSpice (btw. what version?), it is built-in "component", see attached figure VPWL.png. I attached also a part of the manual (zipped pdf).

Best Regards
Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
how to use vpwl in pspice 9.2

mengghee, if you prepare your circuit file (blabla.cir) or netlist (blabla.net) manually, put in the netlist a line similar to the line below but first edit it according to your requirements:

a) substitute the voltage source name "V1" with the proper name in your circuit
b) substitute the "node(+)", "node(-)" with the proper nodes in your circuit
c) substitute the symbols "voltage0", "time1", etc. in the list of time-voltage pairs with required times and voltages

See also the attached figure - the meaning of the time-voltage pairs.
A line in a netlist describing an independent Piece-Wise Linear Voltage source PWL:

V1 node(+) node(-) PWL (0,voltage0) (time1,voltage1) (time2,voltage2) (time3,voltage3) ... etc. (timeN,voltageN)

Good luck ;-),
Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
schematic pspice+ boost converter

Eric, I am using pspice 9.2. i haven't try the things u thought me yet ... but it sounds so complicated as i just learnt pspice a month ago. i'll give it a go. thanks
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
schematic pspice boost converter

mengghee, I have the same version (9.2), so, in my opinion, it shouldn't be complicated to use VPWL for you. You should find VPWL in "source.slb", provided you use PSpice Schematic or in "source.olb" if you use OrCAD Capture as your schematics editor. You simply find and place the component VPWL, then doubleclick on it and edit properties according to your needs and that's it.
If this is the only problem you have, don't give up!

Best Regards
Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
simulation boost converter circuit using pspice

eric,

I have succesfully simulated the schematic with the vpwl. thank you very much. if it's not too troublesome for you, i would like to ask u if you know how to plot a graph of vout vs duty ratio. I would like to plot a graph of my steady state output of my transient analysis vs a varying duty ratio (vpulse). I have been told by my lecturer that this can be done in pspice. i have been trying but in vain. thank you very much
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost pspice schematic

mengghee said:
... how to plot a graph of vout vs duty ratio. I would like to plot a graph of my steady state output of my transient analysis vs a varying duty ratio (vpulse). I have been told by my lecturer that this can be done in pspice. i have been trying but in vain...

It's possible to change the x-axis variable from "Time" to some other variable present in a "blabla.dat", selecting "Plot/Axis Setting.../(button)Axis Variable" in the Probe menu, see the attached figure Axis_Settings.png., but I'm not sure if your 'vpulse' is the case (i.e. variable in .dat), am I right?

Eric
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost converter orcad pspice simulation

continuing:
I think 'vpulse' probably (surely?) IS in the .dat file, but it is in my opinion a PWM waveform which is, I suppose, likely not the point. If I understand your intention well, then the x-axis variable should be rather the duty cycle, i.e. the instant ratio of time intervals with high and low level in 'vpulse' (thus varying number), am I right?

Eric
 

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
pspice simulation for converter

eric,

I have attached a circuit diagram of the boost converter and also the simulation of the output from the comparator opamp (blue),voltage v4 (purple) and sawtooth signal (yellow) . I have used an op amp and a sawtooth to generate the pulse. when i change the voltage at V3, the comparator will generate a different duty cycle. I hope u get what i mean. when i change the value of V4, i also changes the duty cycle. what i want to plot is the Vout Vs Duty cycle (which is also V4). i have tried DC Sweep, but when i use dc sweep. my Y axis of the graph is not the steady state output of my boost. it is some weird answer. so, i assume that i have to use some sort of transient analysis. thank you for ur help. i really appreciate it.
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
boost converter duty cycle graph

mengghee said:
... i have tried DC Sweep, but when i use dc sweep. my Y axis of the graph is not the steady state output of my boost. it is some weird answer. so, i assume that i have to use some sort of transient analysis...

mengghee,
there is no problem to run 'DC Sweep' and 'Transient analysis' at the same time. In the result you obtain 'transient' data for each particular sweep step.

Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
converter pspice

eric,

I have no idea how to do it. and i do not want the whole range of transient analysis data but only the final steady state data. can you tell me how to do it ? thank you very much

mengghee
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
mengghee said:
...I have no idea how to do it. and i do not want the whole range of transient analysis data but only the final steady state data. can you tell me how to do it ?

It's my fault, I'm sorry. It should have been 'transient analysis' together with 'parametric' (it's setup is similar, so I mixed it up).
In transient analysis setup you have to setup No-Print Delay to suppress analysis data from the beginning to the specified time (somewhere before Final time)(your "i do not want the whole range"). Final time must be set 'long' enough for the circuit to reach its steady state, of course (your goal).

In 'parametric' setup choose:
Voltage Source
Name: V3 (the source representing duty cycle)
Sweep Type - Linear
then set up required Start and End Values and Increment.

I suggest to change the sawtooth range from 0 to 1V, the sweep range then mustn't exceed (0V;1V)!, so for instance the sweep parameters can be as follows:
Start Value: 0.05V
End Value: 0.95V
Increment: 0.05V

(The result of the above will be 19 consequential transient analyses.)

Finally change over the noninverting and inverting inputs of OPAMP (just for the analysis purposes), this inverts pwm signal (gate of M1). In such case the value of V3 should be numerically equal to the duty cycle.
Then run this simulation. When finished, select ALL "Available Sections" (just click on OK). (Don't be frightened by so many traces if you had used more voltage or current markers in your schematic ;-))
In the end use (menu) "Trace/Performance Analysis.../Wizard/Next,
choose "YatX" Goal Function, click on Next,
click on the "Name of trace to search" button, choose the required variable, i.e. the output voltage,
write down the "X value to get Y value at" below (say, the Final time value), click on Next and Finish.
You should obtain the required "output voltage vs. duty cycle" graph. If you like, you can delete the plot below clicking on it, i.e. select the lower plot (you can see SEL>> on the left indicating which one is selected at the moment), then (menu) "Plot/Delete Plot. That's it.

Note: it's a good practice, in my opinion, using net labels, preferably mnemonic, e.g. in, pwm, out, etc., then the variables can be easily recognized: V(in), V(out)...

Good Luck ;-)

Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating

mengghee

Full Member level 3
Joined
Nov 29, 2005
Messages
164
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
United Kingdom
Activity points
3,112
eric,

where do i get the 'no print delay' ?? i can't see it anywhere. thank you
 

Eric Best

Member level 4
Joined
Sep 3, 2001
Messages
77
Helped
25
Reputation
50
Reaction score
12
Trophy points
1,288
Activity points
863
mengghee said:
...where do i get the 'no print delay' ?? i can't see it anywhere...

I use PSpice Schematics, your question and pictures of your schematic diagrams indicate you use OrCAD Capture.
I had a look in there and this feature can be found in (menu) "PSpice/Edit Simulation Profile/Analysis - Time Domain (Transient), General Settings, Start saving data after:...seconds.

Eric
 

    mengghee

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top