All About Circuits Forum  

Go Back   All About Circuits Forum > Electronics Forums > General Electronics Chat

Notices

General Electronics Chat Discussion forum for general chat about anything electronics related, including asking questions about material in the All About Circuits E-book, Worksheets, and Videos.

Reply   Post New Thread
 
Thread Tools Display Modes
  #1  
Old 10-24-2011, 02:45 PM
IsoPhaseCore IsoPhaseCore is offline
New Member
 
Join Date: Oct 2011
Posts: 4
Default Importing models into LTSpice, time step too small error

I am trying to import a new model, an AD633 multiplier, and have created a new symbol for it. However, I am getting a 'time step too small' type of error. I've tried increasing the Trtol value (as SgtWookie suggested in an older thread) bringing it up to over 20, but still have the same flavor of error.

Any suggestions? I've attached the model, symbol (had to zip these to get them to attach) and circuit files.

Thank you for your help!
Attached Files
File Type: zip ad633.zip (1.9 KB, 20 views)
File Type: asc Multiplier.asc (1.9 KB, 11 views)
Reply With Quote
  #2  
Old 10-24-2011, 02:47 PM
chrisw1990 chrisw1990 is offline
Senior Member
 
Join Date: Oct 2011
Location: UK, Near Brighton
Posts: 543
Default

i had a problem like this yesterday, it was simply that the circuit stopped working.. crashed if you like.. very odd
__________________
if in doubt.. use a hammer.
Reply With Quote
  #3  
Old 10-24-2011, 03:12 PM
IsoPhaseCore IsoPhaseCore is offline
New Member
 
Join Date: Oct 2011
Posts: 4
Default

I've got it! I followed the advice in this thread:
http://forum.allaboutcircuits.com/sh...ad.php?t=60825

and I was able to get it to work, now I just need to adjust my variable input voltage and current readings (slower time is needed I'm guessing?) to see how the IC reacts.
Reply With Quote
  #4  
Old 10-24-2011, 03:29 PM
IsoPhaseCore IsoPhaseCore is offline
New Member
 
Join Date: Oct 2011
Posts: 4
Default

I'm attaching the files for the 'working' version. However, the simulation is very sensitive to the input values I enter. I'd appreciate if anyone could advise on what Spice settings I could change to help stabilize it (so that I can vary the input in 1 us time frames and test the slew rate / bandwidth of the IC in the model).

Thanks!
Attached Files
File Type: asc Multiplier.asc (1.9 KB, 30 views)
File Type: zip ad633.zip (1.9 KB, 23 views)
Reply With Quote
  #5  
Old 10-24-2011, 03:54 PM
SgtWookie's Avatar
SgtWookie SgtWookie is offline
Expert Member
 
Join Date: Jul 2007
Location: In the vast midwest of the USA; CST
Posts: 22,030
Default

I tried grounding all the inputs (X1, X2, Y1, Y2 and Z), leaving only W connected to ground via a 1k resistor; timestep error.

The only way I could get it to complete running was to leave X1 and Y1 open.

There's something strange going on with that model.

I looked in the Yahoo! LTSpice user group, and found this exchange:

Quote:
> Hi,
>
> I can't get LTSpice to simulate AD633 correctly.
> My output Vout is railed when I used as in the
> schematic posted in the temp folder with the filename
> ad633test.rar
>
> Can someone please help me explain why the model is
> not working correctly? I expect the output Vout to
> be at -9.998V but I am getting it railed to the supply.
>
> Thanks in advance,
>


Hello,

All these multiplier models make a lot of trouble.

Solution for your circuit:
Either only use positive voltages on X1 or exchange the
connection on Y1 and Y2 when you use negative voltages.
You also need the Alternate solver for this circuit.
Control Panel -> SPICE -> Solver:Alternate

Files > Temp > ad633test_GLCc_pos.asc

Best regards,
Helmut
I tried the Alternate solver, and only positive inputs - then only negative inputs. Didn't help.

Another:

Quote:
> Hi
>
> I'm trying to use the AD633 symbols previously discussed
> that are located in Files > Lib > AD633 but i'm having
> the problem that the simulation is extremely slow, a few
> nanoseconds per second. I have uploaded a file where i'm
> trying to use the ad633 for division (per the AD datasheet)
> to the "temp" folder called "ad633extract.asc". Any help
> greatly appreciated! Also i would be very happy to learn
> if there are other ways to perform division within LTSpice?
>
> Thanks
>
> Karl

Hello Karl,

This circuit requires the following settings to run your
circuit with the latest version of LTspiceIV, V4.06?.

1. Use the Alternate solver
Control Panel -> SPICE -> Solver:Alternate

2. You can gain simulation speed.
.options gmin=1e-10 abstol=1e-10 reltol=0.003

Remove or make this SPICE-directive to comment.
.options itl1=500 itl2=500

Files > Temp > ad633extract1.zip

Best regards,
Helmut
I'd tried the different solvers, tried the statements, nothing seems to work except to leave the inputs floating.

Instead of a transient analysis, try a DC analysis.
__________________
General info:
If you have a question, please start a thread/topic. I do not provide gratis assistance via PM nor E-mail, as that would violate the intent of this Board, which is sharing knowledge ... and deprives you of other knowledgeable input.
Reply With Quote
  #6  
Old 10-24-2011, 03:57 PM
SgtWookie's Avatar
SgtWookie SgtWookie is offline
Expert Member
 
Join Date: Jul 2007
Location: In the vast midwest of the USA; CST
Posts: 22,030
Default

Quote:
Originally Posted by IsoPhaseCore View Post
I'm attaching the files for the 'working' version. However, the simulation is very sensitive to the input values I enter. I'd appreciate if anyone could advise on what Spice settings I could change to help stabilize it (so that I can vary the input in 1 us time frames and test the slew rate / bandwidth of the IC in the model).

Thanks!
I didn't see your reply before I posted mine.

Don't bother trying to test the slew rate for this, as it's a macromodel, not a component model. You'll have to go by the specifications in the datasheet.
__________________
General info:
If you have a question, please start a thread/topic. I do not provide gratis assistance via PM nor E-mail, as that would violate the intent of this Board, which is sharing knowledge ... and deprives you of other knowledgeable input.
Reply With Quote
  #7  
Old 10-24-2011, 04:03 PM
IsoPhaseCore IsoPhaseCore is offline
New Member
 
Join Date: Oct 2011
Posts: 4
Default

Hey Sgt, I tried the alternate solver (along with my latest sim settings, and slower input values in posts #2 & 3) and it did help to stabilize the simulation more. It's not perfect, but no model is, and I think it is good enough. Thanks for your help!
Reply With Quote
Reply   Post New Thread

Tags
, , , , , ,


Related Site Pages
Section Title
Textbook Quirks : Using The spice Circuit Simulation Program
Textbook Circuit components : Using The spice Circuit Simulation Program
Textbook Fundamentals of SPICE programming : Using The spice Circuit Simulation Program
Textbook SPICE models : Diodes And Rectifiers


Similar Threads
Thread Thread Starter Forum Replies Last Post
time step too small in ltspice, problem with diode. AbhimanyuSingh The Projects Forum 3 06-25-2011 04:36 AM
Multisim Error zaidqais Electronics Resources 0 08-23-2009 05:54 PM
Measure small time periods with 1ns resolution masteropie General Electronics Chat 9 10-04-2008 01:52 AM
Small error re neutrons in atoms Greg Herrington Feedback and Suggestions 15 02-04-2008 05:05 PM
small error (I think) Unregistered Feedback and Suggestions 9 08-28-2007 07:54 AM

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT. The time now is 12:44 PM.


User-posted content, unless source quoted, is licensed under a Creative Commons Public Domain License.
Powered by vBulletin
Copyright ©2000 - 2014, vBulletin Solutions, Inc.