Multisim and Ultiboard

Showing results for 
Search instead for 
Did you mean: 

RS-485 transceiver spice model

Multisim Experts,
I have been on the hunt for an RS-485 transceiver spice model.  In particular the MAX489, or any comparable full duplex transceiver.  After many hours sorting through web searches I have come up empty handed.  I was able to locate IBIS models for the transceiver, but converting IBIS to Spice using Intusoft's conversion program has been unsuccessful.  I was wondering if anyone knew a good resource on how to write Spice models from existing IBIS parameters or data sheets?  Or if perhaps anyone knew where to locate RS-485 models on the web?
Thanks for your time.
0 Kudos
Message 1 of 7

Do you have the SPICE model that was converted from the IBIS model?  Maybe I can try to get that model work, otherwise you will have to create a circuit that emulates MAX489 using components from Multisim master database.




Tien P.

National Instruments
0 Kudos
Message 2 of 7
 I do have the model that was converted from IBIS.  Saved as an .lib file.  I believe the problem is duplicate subcircuit names or something of that nature.  I am new to creating and modifying SPICE netlists and have been unable to get this model work.  Do you know any good resources (besides whats on the NI site) on this topic?
0 Kudos
Message 3 of 7
If you are not sure how to create a new component in Multisim, refer to this knowledge base:
However, if there is a problem with the SPICE I will not be able to help you without look at it.  Can you zip the file and upload it?
Tien P.

National Instruments
0 Kudos
Message 4 of 7
This is what I have so far... This is the model that was created by the IBIS2SPICE program.  I had attempted to modify some subcircuit name duplicates and was unsuccessful, but his is the original model. 
Thanks for posting the link, though I understand how to create a new component in multisim...My question about resources and information was refering creating the SPICE netlist (from data sheets, IBIS, ect).  I have some info about basic Data statements, control statements, and general anatomy of a spice deck, ect.  but I am looking for more information or books on this topic if you know where to find any.
Thanks again!
0 Kudos
Message 5 of 7

Multisim uses both SPICE and XPSICE simulation engine and there should be plenty of resources available on the Internet relating for these topics.  Here are links where you can find the manuals:






The models you sent me will not work as is, there are minor syntax issues that needs to be modified and for it to work and here is a list:


1.  No 'Param' statements were declared but a couple of statements uses a variable as a value, they did defined variable and was commented out, I guess they expect you to manually change it.  The variables I am referring to are RTR and RTF:


Look for these statements:


*DEFINE {RTR}=  53.731k  ;2.68V/1.44ns

B3 300 850 I= V(830) > 1.2   ? 0 : V(300,850) / {RTR}


Just replace RTR with the value like this:


B3 300 850 I= V(830) > 1.2   ? 0 : V(300,850) / 53.731




2.                  There are many instances where xy_array were used and unfortunately, Multisim does not support this syntax and you need to split the table into x_array and y_array separately.


For example the original model looks like this:

xy_array = [

+   -6.000 ,   -2.360

+   -5.000 ,   -2.360

+   -4.000 ,   -1.800



You need to change it to this:


+ x_array [-6.000 -5.000 -4.000 …..]

+ y_array = [ -2.630 -2.360 -1.800 ….]


3.                  You need to remove the some commas in the model


Original model:


+ fraction = FALSE, input_domain = 0.0,


Change to:

+ fraction = FALSE input_domain = 0.0


4.                  There are several duplicate subckt names declared and you should make them unique.  I simply added an extra number at the end.


The attached file contain the modified model and test circuit, I am not sure what this component is suppose to but I connected some power sources to it and was able to simulate without an error.


I hope this help.



Tien P.

National Instruments
0 Kudos
Message 6 of 7
You have been very helpful.  Thank you for your time. 
Sean P Moorman
0 Kudos
Message 7 of 7