Designer’s Guide Community

shiju

New Member

Offline

Posts: 5

Problem with diode in Hspice
Nov 25^th, 2012, 7:09am

I am trying to simulate a diode using a square wave. code is given below

*diode test
v1 1 0 pulse(0 5 1n 1n 1n 4m 10m)
D1 1 2 D1
.model D1 D()
R1 2 0 1k
.tran 1m 5m
.plot tran v(3)
.end

But when the diode at forward bias, output voltage changes many times. Then I simulate diode with sinusoidal signal, it works properly. Why did this happened and how can I eliminate this?

Back to top

Result.jpg

IP Logged

raja.cedt Senior Fellow Offline Posts: 1516 Germany	Re: Problem with diode in Hspice Reply #1 - Nov 25^th, 2012, 10:48am hello, whats your question? try to draw fig and ask. looks like .plot tran v(3) wrong, becaz there is no node with 3, i guess it is 2. Thanks, Raj.
Back to top	IP Logged

shiju

New Member

Offline

Posts: 5

Re: Problem with diode in Hspice
Reply #2 - Nov 25^th, 2012, 11:51pm

I correct to .plot v(2). But still the problem exist. I explain what is my problem. First I simulate diode with sine wave. Code and result is given below
*diode test
V1 1 0 sin(0 10 500)
D1 1 2 D1
.model D1 D()
R1 2 0 1k
.tran 1m 5m
.plot tran v(2)
.end

Then I simulate same circuit with square wave. code are given below. Result given in my first post.
*diode test
v1 1 0 pulse(0 5 1n 1n 1n 4m 10m)
D1 1 2 D1
.model D1 D()
R1 2 0 1k
.tran 1m 5m
.plot tran v(2)
.end
That at tme 1 to 4ms output voltage changes many times. Thats my problem. what is its reason

Back to top

Result1.jpg

IP Logged

raja.cedt

Senior Fellow

Offline

Posts: 1516
Germany

Re: Problem with diode in Hspice
Reply #3 - Nov 26^th, 2012, 12:14am

hello,
looks like some problem with simulator, try to change some parameter like rise,fall time little bit it may work. There is no problem with your code i ran the same and i got the following result. I guess it's not a problem with diode,otherwise it wouldn't gave correct result with sinusoidal. To make your self happy you could plot diode VI characteristics .

Have fun,
Raj.

Back to top

des.png

« Last Edit: Nov 26^th, 2012, 1:24am by raja.cedt »

IP Logged

shiju New Member Offline Posts: 5	Re: Problem with diode in Hspice Reply #4 - Nov 26^th, 2012, 8:17am My code is work properly in orcad pspice. But it is not working in HSPICE
Back to top	IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: Problem with diode in Hspice Reply #5 - Nov 26^th, 2012, 12:44pm I noticed your AvanWaves version is 4 years old (2008). �Are you using a recent version of HSpice? You might want to add some capacitance to your circuit; some simulators have trouble picking timepoints if there is no dynamic behavior.
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

shiju New Member Offline Posts: 5	Re: Problem with diode in Hspice Reply #6 - Nov 27^th, 2012, 8:11am Yes I am using avanswave 2008. can I get Latest version of Hspice from any website? Can you help me to add capacitance to this circuit. I dont understand fully about what you said.
Back to top	IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: Problem with diode in Hspice Reply #7 - Nov 27^th, 2012, 12:09pm I don't think you can get HSpice from a web site; most places (companies, universities) that have HSpice have a support contract with Synopsys that specifies how/when they get updates. Regarding capacitance, set the CJ parameter: .model D1 D( CJ=1e-12 )
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

shiju New Member Offline Posts: 5	Re: Problem with diode in Hspice Reply #8 - Nov 27^th, 2012, 8:59pm Thank you. It is working.
Back to top	IP Logged