Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Lt spice model for an LM317

Status
Not open for further replies.

user1453

New Member
I've had a look around the web and havn't been able to find an Lt spice model for LM317

does anyone have a model for lm317 or any suggestions for where I might find one?
 
Did you try the LTSpice Yahoo Group?
 
user1453 said:
I've had a look around the web and havn't been able to find an Lt spice model for LM317

does anyone have a model for lm317 or any suggestions for where I might find one?
Here ya go. Unzip this file. Save LM317.sub to the SUB folder in LIB. Save LM317.asy to the MISC folder, which is under the SYM folder in LIB.
 

Attachments

  • lm317.zip
    1.1 KB · Views: 8,271
Does any one have a model for the LM337?

If not is it possible to modify this model so it behaves like an LM337?

Could I just swap the NPN and PNP transistors and diodes over?

Sorry for bumping such an old thread, I just thought it would be easier to post in this one rather creating a new thread.
 
I have this. I don't know if it works.
Code:
*
*LM337 negative voltage regulator
*Connections   Input Adj. Output
.subckt LM337   8       1      19
.MODEL QN NPN (BF=50 TF=1N CJC=1P)
.MODEL QPOUT PNP (BF=50 TF=1N RE=.2 CJC=1P)
.MODEL QP PNP CJC=1P TF=2N
.MODEL DN D
.MODEL D2 D BV=12 IBV=100U
R10 25 6 1K
Q3 8 17 16 QPOUT
Q4 8 25 17 QP
R18 19 17 250
R19 19 16 .3
G1 8 6 1 18 .1
C7 6 2 .04U
R24 2 8 100
I_ADJ 0 1 65U
R26 8 25 200K
Q5 25 4 19 QP
R27 16 4 200
R28 7 4 7K
D1 8 7 D2
D2 8 6 DN
V1 18 19 1.25
.ENDS
 
I'm having problems getting this to work. I think it's me not knowing what I'm doing.

Does this part mean, Input = pin 8, Adj = pin 1 and output = pin 14?
Code:
*Connections   Input Adj. Output
.subckt LM337   8       1      19
I've tried using the 20 pin symbol and it didn't work, I tried using my a modified version of the LM317 symbol and it didn't work.

EDIT:
I've edited it again so it looks the same as the LM317 and it works, so what do those numbers mean?
 
Last edited:
I'm having problems getting this to work. I think it's me not knowing what I'm doing.

Does this part mean, Input = pin 8, Adj = pin 1 and output = pin 14?
Code:
*Connections   Input Adj. Output
.subckt LM337   8       1      19
I've tried using the 20 pin symbol and it didn't work, I tried using my a modified version of the LM317 symbol and it didn't work.

EDIT:
I've edited it again so it looks the same as the LM317 and it works, so what do those numbers mean?
8 1 19 are the numbers of the input, adj, and output, respectively, in the subcircuit netlist. The numbers have no significance. They could have been called manny, moe, and jack, as long as they had the same names in the netlist. What is important is their order. The order corresponds to the PinName and SpiceOrder lines in the .asy file. I have a generic DIP3 symbol (DIP3.asy) that I can use for LM337. LTspice assigns node 8 to pin 1, node 1 to pin 2, and node 19 to pin 3 in that symbol.
I have an LM317 symbol that I (think I) created. I could adapt it to LM337, but have not done so.
 
Last edited:
Here are my LM317 and LM337 symbols.

They're edited versions of your symbol but I added text as I want to use them both in the same circuit and it's less confusing this way.

Thanks to you, the LM337 works now.

Code:
Version 4
SymbolType CELL
RECTANGLE Normal 64 48 -64 -48
TEXT 0 -29 Center 0 LM317
SYMATTR Value LM317
SYMATTR Prefix X
SYMATTR Value2 LM317
SYMATTR Description LM317 voltage regulator
SYMATTR ModelFile LM317.sub
PIN -64 0 LEFT 8
PINATTR PinName IN
PINATTR SpiceOrder 1
PIN 0 48 BOTTOM 8
PINATTR PinName ADJ
PINATTR SpiceOrder 2
PIN 64 0 RIGHT 8
PINATTR PinName OUT
PINATTR SpiceOrder 3

Code:
Version 4
SymbolType CELL
RECTANGLE Normal 64 48 -64 -48
TEXT 0 -29 Center 0 LM337
SYMATTR Value LM337
SYMATTR Prefix X
SYMATTR Value2 LM337
SYMATTR Description LM317 voltage regulator
SYMATTR ModelFile LM337.sub
PIN -64 0 LEFT 8
PINATTR PinName IN
PINATTR SpiceOrder 1
PIN 0 48 BOTTOM 8
PINATTR PinName ADJ
PINATTR SpiceOrder 2
PIN 64 0 RIGHT 8
PINATTR PinName OUT
PINATTR SpiceOrder 3
 
I've had a look around the web and havn't been able to find an Lt spice model for LM317

does anyone have a model for lm317 or any suggestions for where I might find one?
Here ya go. Unzip this file. Save LM317.sub to the SUB folder in LIB. Save LM317.asy to the MISC folder, which is under the SYM folder in LIB.

I have only OrCAD 15.7 Capture CIS Demo from UNI. And i dont know if this LM317 model works with this program. How can i implatet this model.
Sorry for my english :D
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top