Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 
Reply

Components not in multisim libraries

Hi!

I'm an italian high school teacher.

I'm newbie to MultiSim.

I'd like to simulate a PWM interface that use, among others, this two componenents that are'nt in the MS embedded libraries:

  • STMicroelectronics STP10NK60ZFP
  • Optoisolatore uscita transistor 4N35X

I'd like to know wich is the better and faster way to solve the issue:

  1. search and find an equivalent component in the MultiSim library
  2. use a spice model available on the productor's website (if there is one)

I've tried the second way for the mosfet following this tutorial: http://www.ni.com/tutorial/3173/en/

But at step 6 I've received this error message:

 

error.png

I must specify that I'm a mechanical engineer and I teach System and Automation with limited electronic competencies.

Is there anyone that can help me?

Thanks in advance

0 Kudos
Message 1 of 6
(248 Views)

Hi,

searching for your error message I found two forum threads that could give you useful insight:

In the meantime I'll ask NI Multisim experts for advice about the most convenient way to simulate components not present in Multisim embedded libraries.

Regards,

Alessia

0 Kudos
Message 2 of 6
(209 Views)

Hi. Alessia.

This is a very important issue for me.

Thanks in advance

0 Kudos
Message 3 of 6
(200 Views)

Hi,

it seems you made a mistake in one of the first steps in the Component Wizard; you defined a symbol to use on the schematics having 3 pins (component symbol pins), but the SPICE code defines 5 inputs/outputs (model pins). That does not match up. I'd guess you picked a symbol with only three pins in step 3 of the wizard.

If you can't figure it out, could you please attach the component file? Otherwise I'm afraid I can't help you that much.

Regards,

Alessia

0 Kudos
Message 4 of 6
(195 Views)

Hi alamanna, thansk for your reply.

I've downloaded the model directly from the ST website:

https://www.st.com/content/st_com/en/search.html#q=STP10NK60ZFP-t=resources-page=1

Attached to this mail the downloaded model.

Otherwise, if I look on the ST website, I can see that the component has only 3 pins:

 

STP10NK60ZFP.png

 

Any idea?

Thanks in advance,

0 Kudos
Message 5 of 6
(171 Views)
Highlighted

Hello mforbiz,

I had a look at the SPICE model you attached and the SPICE code itself also defines three parameters/pins (named 1, 2, and 3 in the .SUBCKT definition), so that's fine:

* MODELLING FOR STP10NK60ZFP
.SUBCKT STP10NK60ZFP 1 2 3
LG 2 4  7.5n
[...]

 

I tried the steps of importing the model into Multisim myself...

2019-04-17_13-55-35.png

 

and found the cause: The comment in the first line confuses Multisim. Remove it and it works:

multisim_2019-04-17_13-56-56.pngComment removed.multisim_2019-04-17_13-57-11.pngSuccessfully proceeded to next step.

 

 

Edit: I am using Multisim 14.1.0. I did some further testing and found the issue being correlated to the comment containing the model name.

This is fine:

 

* This is a comment
.SUBCKT testik 1 2
R 1 2 2K
.ENDS testik

 

This errs out:

* This is testikabcd a comment
.SUBCKT testik 1 2
R 1 2 2K
.ENDS testik

 

 


Ingo – LabVIEW 2013, 2014, 2015, 2016, 2017, 2018, NXG 2.0, 2.1, 3.0
CLADMSD
Message 6 of 6
(141 Views)