Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

Simulation Error on Agilent/Tektronix Oscilloscope

Hi there,

Recently, for academics purpose, I just design the half-wave power supply circuit .I've been trying to use Agilent and Tektronix Oscilloscope provided by MultiSim 9 to show the output (see attachment). After a few second (about 2.76 sec) there come the message :

|   Instrument Analysis: Transient Analysis  
|   |   Plot title:
|   |   Analysis settings
|   |   |   Initial Conditions: Automatically generate initial conditions
|   |   |   Starting time (TSTART): 0
|   |   |   Stop time (TSTOP): 1e+030
|   |   |   Plotting increment (TSTEP): automatically calculated (less than: 1e+030)
|   |   |   Maximum time step (TMAX): automatically calculated (less than: 1e+030) 
|   |   Perform consistency check
|   |   Variables from analysis  
|   |   |   Show device values at the end of the simulation  
|   |   Representation as SPICE commands
|   |   |   begin-scope page
|   |   |   checknodes 3
|   |   |   save all
|   |   |   iplot all
|   |   |   set trtol = 7
|   |   |   set itl4 = 100 
|   |   |   set convlimit
|   |   |   set rshunt = 1e+012  
|   |   |   -param hrange 0 1e+030 
|   |   |   save
|   |   |   tran  -env-options 1e-005 1e+030 0 1e-005 auto_ic auto_tstep auto_tmax 
|   |   |   if-error end-scope audit-log-show
|   |   |   show all
|   |   |   showmod all  
|   |   |   end-scope
|   |   Multisim Default Analysis Options
|   |   |   Truncation error overestimation factor: 7
|   |   |   Upper transient iteration limit: 100
|   |   |   Enable convergence assistance for code models
|   |   |   Shunt resistance from analog nodes to ground: 1e+012
|   Output from instrument analysis  
|   |   TRAN:  Timestep too small; time = 2.76, timestep = 1.23789e-015: trouble with node $6:xt1
|   |   doAnalyses: timestep too small 
|   |  
|   |  
|   |   tran simulation(s) aborted 


I don't know what happen, but if I change with the "original type" of oscilloscope from the instrument toolbar, the simulation works fine. I also trying to search for node $6:xt1 as written in the message, but I got nothing. What is the meaning of this node and how to find the related node on the circuit ?

Could someone help me ?

Ghost Recon Team Leader
Ghost Recon Team Leader
0 Kudos
Message 1 of 5
(5,354 Views)

Hi,

 

For information how to fix time step too small errors, view the knowledge base from the link shown below:

http://digital.ni.com/public.nsf/allkb/4B99B2CD6C0C3B6A86257205005D58E0

I got your circuit to work by changing the follow:

Tmax from 1e-5 to 1e-3 sec

Reltol from 0.001 to 0.01

Rshunt from 1e+12 to 1E+7

And Integration method from Trapezoidal to Gear.

 

Tien

Tien P.

National Instruments
0 Kudos
Message 2 of 5
(5,332 Views)
Hi Tien, thanks a lot for the advice. I just followed up your link and change to "Set to zero" for the initial condition. And, yup, it works !!

Unfortunately, I need more help from you. I use three methods for the measurement. Tektronix, Agilent and Probe (see attachment). I want to measure Vp-p, Vdc and Vrms for the output. The differencies come with the value of Vrms. While Tek's and Agi's using

Vrms=sqrt ( (Vp-p/2)^2 - (Vp-p/phi)^2 ) = 0.385 * Vp-p --> in this case Vrms=0.385 * 26.2 = 10.1V



But, the probe use

Vrms = Vp-p/2 --> in this case Vrms=12.9 V

I'm not very sure, but for me it seems there is a "big" differency between 10.1 and 12.9.....around 2 volts !!


So, which one is the best ?

Ghost Recon Team Leader

Ghost Recon Team Leader
0 Kudos
Message 3 of 5
(5,297 Views)

Multisim calculates RMS in two ways:

1.  It removes the DC offset and from the signal and then calculate the RMS value, instruments uses this method.

2.  The other method is to leave DC off set vale and then calculate the RMS value, probe uses this method.

 

In this example, I have an AC source with a 1V DC offset, from the result you can see the probe RMS value being higher than the meter reading due to the 1 V DC value.

 

 

Tien P.

National Instruments
0 Kudos
Message 4 of 5
(5,285 Views)
Thanx again Tien. Got u'r point now !
Ghost Recon Team Leader
0 Kudos
Message 5 of 5
(5,265 Views)