RS-485 transceive​r spice model

Question

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.

Answer 1

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:
SPICE:
http://esaki.ee.boun.edu.tr/~talays/spice/spice.pd​f
XSPICE:
http://users.ece.gatech.edu/~mrichard/Xspice/Xspic​e_Users_Manual.pdf
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
Tien P.
National Instruments
Attachments:
RS-485.zip ‏82 KB