The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Simulators >> Circuit Simulators >> Problem with diode in Hspice https://designers-guide.org/forum/YaBB.pl?num=1353856180 Message started by shiju on Nov 25th, 2012, 7:09am |
Title: Problem with diode in Hspice Post by shiju on Nov 25th, 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? |
Title: Re: Problem with diode in Hspice Post by raja.cedt on Nov 25th, 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. |
Title: Re: Problem with diode in Hspice Post by shiju on Nov 25th, 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 |
Title: Re: Problem with diode in Hspice Post by raja.cedt on Nov 26th, 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. |
Title: Re: Problem with diode in Hspice Post by shiju on Nov 26th, 2012, 8:17am My code is work properly in orcad pspice. But it is not working in HSPICE |
Title: Re: Problem with diode in Hspice Post by Geoffrey_Coram on Nov 26th, 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. |
Title: Re: Problem with diode in Hspice Post by shiju on Nov 27th, 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. |
Title: Re: Problem with diode in Hspice Post by Geoffrey_Coram on Nov 27th, 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 ) |
Title: Re: Problem with diode in Hspice Post by shiju on Nov 27th, 2012, 8:59pm Thank you. It is working. |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |