Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

Looking for MC1496 - any custom part library?

Solved!
Go to solution
Highlighted

Hey all,

 

I'm trying to simulate the signal modulator/demodulator chip MC1496. It seems it doesn't come standard with Multisim. I was wondering if there was as custom parts library that the community has put together (or something of the sort).

 

I have the part for LTSPICE but (seeing as how I've been using Multisim for a grand total of half an hour) am not completely confident in my abilities to get it imported and set up correctly. If someone else more experienced with Multisim than I has already done it that would be infinitely preferable.

 

Thanks a lot.

0 Kudos
Message 1 of 27
(16,167 Views)

Hi,

 

Have a look at this link:

http://www.doe.carleton.ca/~cp/telecom/mixer.txt

 

This the MC1496 model is part of the circuit netlist and this is the section you want:

 

 Mixer Subcircuit
* See figure 23 of data sheet with following modification to 
* reflect Metal Can instead of DIP package
* Pin # fig23   subckt
*        9       12
*        8       10
*        7       8
*        10      14
.subckt MC1496 1 2 3 4 5 6 8 10 12 14
* Tail current Source
Q1 3  5  19 Q2n3904
Q2 2  5  13 Q2n3904
* Input transistors
Q3 7  4  3  Q2n3904
Q4 9  1  2  Q2n3904
*LO quad switching Transistors
Q5 6  8  7  Q2n3904
Q6 6  10 9  Q2n3904
Q7 12 10 7  Q2n3904
Q8 12 8  9  Q2n3904
* Emitter degeneration resistors
RE1 19 14 500
RE2 13 14 500
*
* Current Mirror
Q9 5  5 15 Q2n3904
Rd  15 14 500 
.ENDS

 

If you don't know how to create a component in Multisim, have a look at this tutorial:

http://zone.ni.com/devzone/cda/tut/p/id/3173

 

 I didn't test this model but I hope it will work for you.

Tien P.

National Instruments
0 Kudos
Message 2 of 27
(16,097 Views)

Thanks for the advice Tien. I figure this must be the right spice model as it is very similar to other leads I have found. However, I still can't get the part to work. I think perhaps I am setting it up wrong - the custom component guide is pretty confusing.

 

It mentions that parts with multiple internal components (like op-amps) are multisection components. Initially I would think that this device with 8 internal transistor would qualify, but I'm not sure.

 

I also think that perhaps the most likely reason it is not working is due to errors in the mapping between the symbol nodes and the model nodes. The comments in the subckt are not nearly as helpful as those in the guide example. I cannot figure out what the symbol nodes correspond to in the model, nor can I decifer the model to figure out what the lines are referring to.

 

It mentions "Figure 23" in the datasheet, which I believe refers to figure 23 in MC1496 datasheet. That is the same as this image (taken from the device application note).

 

18649iA5C53BD5E5268F1B

I know the "tail current source" is (from the schematic) transistors Q7 and Q8, the "input transistors" are Q5 and Q6, and the "LO quad switching Transistors" are Q1-Q4. But as for figuring out the link between this graphic and the subckt nodes, and linking that to the symbol file in Multisim, I am at a loss.

 

I could really use this for my project. Any more advice you have would be greatly appreciated. Thanks.

0 Kudos
Message 3 of 27
(16,048 Views)

After analyzing the spice file and the diagram a little more, I *think* everything is in the right place. I still don't understand why my circuit refuses to work, however. I've attached my project file, which is the MC1496 wired up in "Figure 27 - AM Modulation Circuit" configuration from the datasheet. If you have any idea where I went wrong, please let me know.

0 Kudos
Message 4 of 27
(16,041 Views)

I am also getting the following error in my simulations:

 

 

------ Checking SPICE netlist for MC1496 - 2010-07-12 11:42:14 ------ 
SPICE Netlist Error in schematic RefDes 'u1', element 'xu1':  Unable to interpret 'u1_open_11'
======= SPICE Netlist check completed, 1 error(s), 0 warning(s) ======= 

 

------ Checking SPICE netlist for MC1496 - 2010-07-12 11:42:14 ------

 SPICE Netlist Error in schematic RefDes 'u1', element 'xu1':  Unable to interpret 'u1_open_11

'======= SPICE Netlist check completed, 1 error(s), 0 warning(s) ======= 

 

Where U1 is my modulator chip.

0 Kudos
Message 5 of 27
(16,037 Views)
Solution
Accepted by topic author strugglingEngineeringStudent

As far as I can tell here, the problem is the pin mapping between the symbol and the model. The .subckt only uses 10 pins, but the symbol has 14. In the symbol to model pin mapping, you have the default assignment - all 14 symbol pins assigned to model nodes.

 

Based on the .subckt line and the way you have the component wired in to the schematic, it looks like pins 7, 9, 11, and 13 are unused. You'll need to set those as "Not Connected" (NC) in the mapping table, and adjust the remaining pins appropriately (symbol pin 8 will actually be the 7th model node, pin 10 is the 8th node, pin 12 the 9th node and pin 14 will be the 10th node - conveniently this subcircuit uses the pins in order, it just skips a few).

 

That should fix the simulation error. The error was just because it was trying to use 14 nodes for a 10 node .subckt. (u1_open_11 is just the name that was assigned to pin 11's simulation node because the model mapping said to use it, but there's nothing connected).

Christopher Lansing
Software Developer
National Instruments
Message 6 of 27
(16,024 Views)

I followed your advice to the letter and it works! Thanks a million. I am very impressed with the level of dedication to the userbase displayed here. If a paper comes from this project, you two will definitely be receiving a mention in the acknowledgements section

0 Kudos
Message 7 of 27
(16,000 Views)

Neat! Please post a link to your project/paper here too (if possible). We are always interested to see what our users are doing!

----------
Yi
Software Developer
National Instruments - Electronics Workbench Group
0 Kudos
Message 8 of 27
(15,972 Views)
0 Kudos
Message 9 of 27
(15,393 Views)

Sorry, but how can i do that, i use the code up to generate a part but i can't set the pins to Not Connected.

0 Kudos
Message 10 of 27
(14,669 Views)