PSpice Ideal Diode ... and Crash
Bookmark this page:
 Yahoo!
 Google
 Windows Live
 del.icio.us
 digg
 Netscape
|
|
||||||||||||||||||||||||||||||||||||||||
|
Posted by Jim Thompson on October 15, 2005, 12:28 pm
Please log in for more thread options On Sat, 15 Oct 2005 12:03:54 -0700, Bob Penoyer >>On Thu, 13 Oct 2005 19:57:30 -0700, Bob Penoyer
>> >>>On Thu, 13 Oct 2005 07:44:26 -0700, Jim Thompson
>>> >>[snip]
>>>>
>>>>Do you perchance have two (or more) versions of PSpice installed? >>> >>>No. I'm using one of the "seats" that the license allows. >>> >>[snip]
>> >>Make sure there isn't more than one version on your machine. That'll >>screw you up every time. >> >>From support... >> >>"The problem you have mentioned in your email regarding the simulation >>error is something that can be caused if the user has multiple >>versions on the system or he still has old version entries in the >>environment variables and registry. This happens only with Capture and >>not with PSpice Schematics." >
>This is very interesting. I'm sure (I think...) that I uninstalled >anything related before installing. Maybe I should go through the >process again. Might be worth a try, but I did previously post some bugs in 9.x that were fixed in 10.x that looked like possible culprits. ...Jim Thompson -- | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | | http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food. | ||||||||||||||||||||||||||||||||||||||||
|
Posted by Helmut Sennewald on October 13, 2005, 9:43 pm
Please log in for more thread options >I recently had a need for an ideal diode. When I found one and used
http://ocw.mit.edu/NR/rdonlyres/Electrical-Engineering-and-Computer-Science/6-334Spring2003/56F6E619-0B02-424D-AC10-88D1AC4AB3E1/0/idealdiode.lib
> it, I got results that worked great in one circuit and crashed PSpice > in another circuit. I've had convergence problems before, but never a > crash. > > I found a model for an ideal diode at this MIT site: > Hello Bob, This model uses an extreme low value of N=0.001 in the diode model. The diode equation looks like Id = Is*exp(V/(N*Vt)) It's obvious that this small value of N can cause very big exponents if the equation solver in SPICE makes too big steps. This can lead to a math overflow. Neverthess a good program shouldn't crash in this case. You could also try with a bigger value like N=0.005 or maybe adding a small series resistance parameter RS=0.01 may help. Btw, it's nonsense to make a subcircuit around a simple .model statement. Other SPICE programs may or may not have problems with this extreme paramter value. It's just a question if the programmers had such values in mind or not. LTspice works with this diode model. I recommend you send your test case to Cadence and ask for "bug" fix. Best regards, Helmut The model from the link above. ************************************************************************ **** diode_ideal (approximates ideal diode) **** ************************************************************************ ..subckt diode_ideal 1 2 D12 1 2 diode_ideal ..model diode_ideal D (N=0.001) ..ends diode_ideal ******************************************************* | ||||||||||||||||||||||||||||||||||||||||
|
Posted by Bob Penoyer on October 13, 2005, 8:27 pm
Please log in for more thread options
On Thu, 13 Oct 2005 21:43:17 +0200, "Helmut Sennewald" >>I recently had a need for an ideal diode. When I found one and used
http://ocw.mit.edu/NR/rdonlyres/Electrical-Engineering-and-Computer-Science/6-334Spring2003/56F6E619-0B02-424D-AC10-88D1AC4AB3E1/0/idealdiode.lib
>> it, I got results that worked great in one circuit and crashed PSpice >> in another circuit. I've had convergence problems before, but never a >> crash. >> >> I found a model for an ideal diode at this MIT site: >> >
> >Hello Bob, > >This model uses an extreme low value of N=0.001 in the diode model. >The diode equation looks like > >Id = Is*exp(V/(N*Vt)) > >It's obvious that this small value of N can cause very big >exponents if the equation solver in SPICE makes too big steps. >This can lead to a math overflow. Neverthess a good program >shouldn't crash in this case. You could also try with a >bigger value like N=0.005 or maybe adding a small series >resistance parameter RS=0.01 may help. > >Btw, it's nonsense to make a subcircuit around a simple .model >statement. I'm not sure why. The MIT site did it. What's the problem? In any case, I used a single .model statement in Model Editor which is pretty common. | ||||||||||||||||||||||||||||||||||||||||
|
Posted by Helmut Sennewald on October 14, 2005, 7:26 am
Please log in for more thread options
> On Thu, 13 Oct 2005 21:43:17 +0200, "Helmut Sennewald"
> >>>I recently had a need for an ideal diode. When I found one and used
http://ocw.mit.edu/NR/rdonlyres/Electrical-Engineering-and-Computer-Science/6-334Spring2003/56F6E619-0B02-424D-AC10-88D1AC4AB3E1/0/idealdiode.lib
>>> it, I got results that worked great in one circuit and crashed PSpice >>> in another circuit. I've had convergence problems before, but never a >>> crash. >>> >>> I found a model for an ideal diode at this MIT site: >>> >>
>> >>Hello Bob, >> >>This model uses an extreme low value of N=0.001 in the diode model. >>The diode equation looks like >> >>Id = Is*exp(V/(N*Vt)) >> >>It's obvious that this small value of N can cause very big >>exponents if the equation solver in SPICE makes too big steps. >>This can lead to a math overflow. Neverthess a good program >>shouldn't crash in this case. You could also try with a >>bigger value like N=0.005 or maybe adding a small series >>resistance parameter RS=0.01 may help. >> >>Btw, it's nonsense to make a subcircuit around a simple .model >>statement. >
> I'm not sure why. The MIT site did it. What's the problem? Hello Bob, I haven't said it doesn't work with the .subckt, but it's not necessary. It has the drawback that SPICE eventually makes a bigger matrix. > In any case, I used a single .model statement in Model Editor which is
> pretty common. Best regards, Helmut | ||||||||||||||||||||||||||||||||||||||||
|
Posted by Bob Penoyer on October 15, 2005, 12:01 pm
Please log in for more thread options
On Fri, 14 Oct 2005 07:26:45 +0200, "Helmut Sennewald" >>>Btw, it's nonsense to make a subcircuit around a simple .model
>>>statement. >>
>> I'm not sure why. The MIT site did it. What's the problem? >
>Hello Bob, > >I haven't said it doesn't work with the .subckt, but it's not >necessary. It has the drawback that SPICE eventually makes >a bigger matrix. Okay, Helmut. Thanks. | ||||||||||||||||||||||||||||||||||||||||
| Similar Threads | Posted |
| PSpice Ideal Diode ... and Crash | October 12, 2005, 9:10 pm |
| Convert HSpice Diode Model to PSpice? | March 28, 2007, 12:02 pm |
| diode voltage | February 8, 2008, 11:09 am |
| diode 1n4733 | May 2, 2008, 11:04 am |
| System crash in 99SE | June 28, 2007, 2:22 pm |
| Wine and LTspice crash | January 23, 2006, 6:47 pm |
| Re: Tri to Sine diode shaper | June 13, 2008, 1:57 am |
| Re: Tri to Sine diode shaper | June 12, 2008, 12:53 pm |
| Re: Tri to Sine diode shaper | June 16, 2008, 11:53 am |
| diode protection in battery charger circuit? | July 17, 2008, 1:36 am |
| diode protection in battery charger circuit? | July 17, 2008, 1:34 am |
| new to pspice | September 14, 2004, 12:24 pm |
| Pspice | November 18, 2004, 4:15 pm |
| Is Pspice very useful? | October 30, 2006, 8:22 pm |
| Pspice? | November 15, 2006, 1:08 am |
>