Multisim and Ultiboard

Showing results for 
Search instead for 
Did you mean: 

opening switch

opening switch

I am a 3-hour old Multisim user.
How can I insert opening switch with close/open resistance and open/transition time in Multisim?
With Pspice, this was easy by changing Rclosed, Ropen, Topen, and Ttran.


0 Kudos
Message 1 of 11

Re: opening switch

Hi jim612,
If I understand the question right, then you need to place down a component from the electro mechanical group.
You are looking for switches in there?
If that isn't what you are looking for then go to the Basic group and you are looking for the switches in there?
Is that what you are looking for?
Applications Engineering Team Leader | National Instruments | UK & Ireland
0 Kudos
Message 2 of 11

Re: opening switch

I am currently testing both Pspice and EWB for our purpose.  I am trying to simulate a circuit with hypothetical opening switch.  With Pspice, I was able to include opening switch  "Sw_tOpen" with properties
"tOpen=2.24us ttran=.1ns Rclosed=1m Ropen=1Meg" to simulate open time, transition time from closed resistance to open resistance.  I can do this by right clicking switch and changing properties in Pspice.  I think Sw_tOpen is Spice3 part.
In the basic group of multisim, I found a switch (SPST?).  But how can I change parameters or attributes?
0 Kudos
Message 3 of 11

Re: opening switch

The majority of switches in Multisim are actually interactive, so when you are simulating you can hit a reserved key on the keyboard to open-and-close a switch as necessary. This is different from pSPICE which does not offer that ability to interactively access components during simulation.
If however you need a switch that will only be on for pre-defined amounts of time, I suggest using:
1.) Place >> Component
2.) Database = Master Database, Group = Basic, Family = Switch
3.) Select the TD_SW1 switch
If you double-click on this switch, you can define how long the switch will be on and off.
Message 4 of 11

Re: opening switch

Thanks for reply.

However, what I am trying to do is a little bit more complicated than simple timed switch on/off. I would like to specify resistance when switch is on or off and also transition time from on to off state. No realistic switch can open in "zero" time. No realistic switch can have zero/infinite resistance in on/off state. I want to study transient circuit response when these switch parameters varies. What do I have to do to simulate this realistic switch in EWB? Here is one site with good PSPICE example:

Switch U1 in Example 1 is what I want.


0 Kudos
Message 5 of 11

Re: opening switch

You would have to copy the switch from the master library and put it in the user library. From there you would have to edit the modeling data to include the transient time and switch resistance values. Or you could create a custom component switch and program the model yourself (which is time consuming).

Either way it will take time to do what your asking.

Signature: Looking for a footprint, component, model? Might be here >
0 Kudos
Message 6 of 11

Re: opening switch

I have a similar problem pertaining to the operation of the switches in the ns range. The sitch works fine when the on and off time are set in the ms range, but when set in the ns or us range the switch does not respond. Any solution.
0 Kudos
Message 7 of 11

Re: opening switch


I have a switch question too.. Is it possible to simulate switches in the transient analysis? I included some simple timed switches in some of the circuits, but I can't get Multisim to simulate this in transient analysis.

Tnx for any help.
0 Kudos
Message 8 of 11

Re: opening switch

The time delay switch is an interactive component, that means when you run the simulation in the regular mode, you can see the switch switching on the screen.  This is not a SPICE native property so when you import it into the transient analysis, it does not work. 


To work around this, you can create a SPICE native model and the switch should change state in middle of the analysis.  Below is a model to emulate the time delay switch:


.subckt TD S1 S2

xU2 1 0 S1 S2 SW

xU1 1 0 PWL

.subckt SW   1 2 3 4

S1  3  4  1 2   vsw

.model vsw sw (

+                  vt    = 0.001

+                  vh    = -1e-006

+                  ron   = 0.001

+                  roff  = 1e+009

+                )


.subckt PWL 1 2

V1 1 0 PWL (0,0) (0.01,0) (0.01001,10)




The model is made up of two basic SPICE components, a PWL and a voltage control switch.


The body of the PWL is here:

V1 1 0 PWL (0,0) (0.01,0) (0.01001,10)

(0,0)àtime 0 voltage is 0V

(0.01,0) >> t=0.01, V= 0

(0.01001,10) >> t=0.01001 V=10


The PWL is a “connect the dot” component and in this example, I gave it three points.


The second part of the model is a Volt control switch.  When the voltage crosses the 0.001V it changes state.


 I also made a circuit to show what this model looks like in a schematic.



Message 9 of 11

Re: opening switch


Thank you for your reply, it is quite useful!

However, this approach is still somewhat unpractical as it is confusing to put circuits like this to replace every switch. It tried saving it as a HB and duplicating it but when you change properties ("openning" time) of one, all of them change. Is it possible to contruct an independent component this way?
I hope I am not asking things too obvious, but I am not an electronics expert, skillful with Multisim - even less Smiley Happy.

0 Kudos
Message 10 of 11