Spice model 2n2646

[Dervakon]

Hi everybody,

How I can make a spice model for UJT 2N2646 I found one but it's not working... or were I can fin one. I know we don't use that kind of transitor anymore but I need it for school...

Thx

[lacy]

I hate to reply to your question this manner, but have your tied to Google for it? Just put in "UJT 2N2646 Spice Model" and something should pop up. This is no sign that the model will work in Multisim. You will just have to keep plugging models in until you find one that works. It took me forever to find a model for an IC that worked and even then it wasn't the exact same IC but something simular.

Good luck in your hunt. This is why we Multisim users need a free Part Models Website. Are you listening NI?

[lacy]

I just tried a Google search just to be funny and I found diddly squat. After making my last post I remembered that I had done an exhuastive search for UJTs a couple months ago. I found one (and this may be the only one.) I have posted it below with the website where I found it to give them credit for the model. I haven't tried these models so I do not know if they work or not. Give them a shot and see what happens.

* http://www.duncanamps.com/spice/miscsemi/2n2646.sub
*
*Default N-Channel Unijunction Transistor
.SUBCKT XUJT 1 2 3
DE 1 4 EMITTER
VE 4 5 DC 0
HVE 6 0 VE 1K
RVE 0 6 1MEG
BBB 5 7 I=0.00028*V(5,7)+0.00575*V(5,7)*V(6)
CBB 5 7 35P
***RB1 7 2 38.15 RMOD
***RB2 3 5 2.518K RMOD
RB1 7 2 RMOD 38.15
RB2 3 5 RMOD 2.518K
.MODEL RMOD R TC1=.01
.MODEL EMITTER D (IS=21.3P N=1.8)
.ENDS XUJT

* Motorola IP=.5U IV=6M VB1(sat)=3 Rbb=6.1K Vob1=3.6: E, B1, B2
.SUBCKT X2N2646 1 2 3
DE 1 4 EMITTER
VE 4 5 DC 0
HVE 6 0 VE 1K
RVE 0 6 1MEG
BBB 5 7 I=0.00028*V(5,7)+0.00575*V(5,7)*V(6)
CBB 5 7 35P
***RB1 7 2 38.15 RMOD
***RB2 3 5 2.518K RMOD
RB1 7 2 RMOD 38.15
RB2 3 5  RMOD 2.518K
.MODEL RMOD R TC1=.01
.MODEL EMITTER D (IS=21.3P N=1.8)
.ENDS X2N2646

[nestor-sg]

I recently came across someone asking for the same component. Together with Lacy's-provided link and the Philips datasheet, I created the 2N2646 component. I can't tell for sure if the SPICE code is accurate or not, since the only circuit I have handy is the test circuit from the Philips datasheet and have no results to compare. Please check it out and see if the code is accurate or not. Attached is a zip file with:

• Schematic.pdf: Just a schematic printout of 2N2646.ms11 showing the test circuit from Philips and the response I got from the oscilloscope and the transient analysis using the "duncanamps" SPICE code.
• 2N2646.ms11: Multisim 11 schematic with the component. You can right-click Q1 and select "Save component to DB..." and may I suggest saving in Corporate DB > Transistors > and create a UJT family. You may want to later go to the Database Manager and make this family have a default Q prefix (it will use U as default when newly created).
• 2N2646.ewprj: Ultiboard 11 layout file, the only part in this file is a modified version of the TO-18 package since the one shown in Philips datasheet is different (in form and pin order) than the one in Ultiboard.

I hope this is useful for those of you that have requested this component in the past.

Cheers,

Message Edited by nestor on 06-03-2010 08:39 PM

[Just_Plain_Bob]

Gentlemen,

2n2646 aren't necessarily spec'd for new designs, but they are available for about $2 apiece from Newark. The point is, they ARE still used. There's plenty of legacy circuits using that part (along with many other older parts that don't appear in Msim libs) and they're still valid for use.

The main point of this interjection is, however, the 10th edition, 11ed etc of school lab manuals still use the same parts that were in the 2nd edition. It's extremely frustrating trying to find these parts or similar parameter components in order to complete the labs. Now, you may blame the text authors for not updating their materials (I do). On the other hand, Msim ACADEMIC VERSION purchased as a requirement for many of these school programs might be friendlier to the students required to make the purchase if, in addition to the standard component database, ALSO INCLUDED these older parts that show up in the lab manuals! eg, ujt 2646, scr2326 I think, 1n43A diode, 2n3053 med pwr transistor, LM3914 etc etc. Would NI like a copy of some of the lab manual pages in question to get an idea of the parts lists that students can never find in Msim? I'm older than most of these parts and I don't think old is bad....  🙂

Change subject: Lacy, I have some homemade subckts in my user db that some users might find useful. How can I export the individual part so that the uploaded component file has all the required info including symbol and footprint? One example is R or RC networks SIP package with generic SIP footprint so it can be shown on a pcb layout. I didn't really want to send my whole user db to your site.

Bob

[Mark J]

I have some questions and some answers.

We definitely understand that there are legacy components that our users would like included in our software. Unfortunately, we can't always deliver simulatable legacy components. Often component manufacturers have not created models for these old components, or they have purposefully obsoleted them and have long since stopped distributing the model.

We have been working to increase the scope and breadth of our database with simulatable components that have models directly from the manufacturer. This includes recent additions from Analaog Devices, Linear Technologies, Microchip, National Semiconductor, and Texas Instruments. There are more to follow.

With regards to the components that you list, are you primarly interested in simulation, layout, or both? I'm assuming from the context of this thread that the focus is on simulatable components. For example, you mention the LM3914 from National Semiconductor. Are you interested in having this component with a simulation model, or is this for schematic capture and layout purposes only?

As for questions about lab manuals and curriculum. If you have a list of these components from lab manuals, we would certainly like to take a look at it. Perhaps you can work with Nestor to send us this material.

Thanks,

Mark

[Just_Plain_Bob]

Mark

I would be happy to scan pages and forward to an email address (authors may not like their material posted for general distribution). One of the texts is Electronic Devices and Circuit Theory 10th & 11th editions by Boylestad. Like mentioned above, I've seen other students looking for parts in forums over the past two years. Many are lost as to how to find a similar component since they are new students.Some schools switched from microcap to msim but neglected to determine the effect through a review the textbooks. I've acted as a sort of virtual lab assistant for some of the professors while taking their courses and helped students where I could with substitute components, finding an esoteric model out on the net, or explaining that concepts were what was important rather than the specific parts used and I would supply suitable ms10 files and instructions.

The most prevalent student responses gathered from many student email exchanges are:

1. blame the professor

2. blame and diss Msim

It would be nice to have new students (potentially full blown NI products users) not dissing Msim and being left with a bad taste.

However, sometimes the purpose of finding the older components is to simulate legacy circuits in order to characterize overall circuit parameters and find suitable replacement designs. It is still a good idea to:

1. locate a validated parametric part model.

2. create an unvalidated model from a datasheet

3. create a subckt with equivalent functionality made from different parts of course (eg LM3914)

4. use an ABM if plausible (eg LM3914?)

The schematic symbol with correct pinout for simulation, and footprint would be desired. The footprint would be based on THC versions rather than only SMC since things are often breadboarded. For something like the LM3914, I may be wrong but I don't think there is a parametric spice model to be had. I am creating a 'functional equivalent' as a subcircuit and will use the dip package pinout and footprint.I haven't explored the use of an ABM for this yet.

bob

[qirxaz]

thank you for this piece

[Just_Plain_Bob]

Q

You are certainly welcome!. This has been a long standing issue with me. (college text books, mandatory purchase of msim, no harmonization between textbook requirements and msim resources). Kind of like federal requirements put on states without the federal funding to follow the requirements....

Nevertheless, Msim is my favorite. If it would only stop giving me repetitive simulation errors while Convergence Assistant says it can't reproduce the error....  I like Convergence Assistant feature otherwise. Nice touch.

I'm about to send in a rather mundane circuit where this is occuring (new thread).

Bob (JPB).

[aesanchez]

Hi

I have tried this model in OrCAD PSpice 16.3 and found several problems,

1. .MODEL RMOD R TC1=.01 Gives invalid model type, I changed it to .MODEL RMOD RES(R=1,TC1=0.01) which gives no error.

2. BBB 5 7 I=0.00028*V(5,7)+0.00575*V(5,7)*V(6,0) is an invalid parameter. I reviewed all literature of spice for this line and could not find anywhere, where this statement is correct. I did found however it might be posible to implement this function using the POLY statement.

Has anybody have succesfully implemented this model in PSpice?

Regards

Alberto