LTSpice SCR simulation help - Page 1
Forum section: electronics / projects

author: anishkgt
author_rank: Frequent Contributor
timestamp: September 26, 2017, 10:01:29 am
content: Hi All,I am trying to simulate an scr working for determining snubber values. I just can get the parameters correct for it to work.Would appreciate if anybody could help me resolve this error.

author: Ian.M
author_rank: Super Contributor
timestamp: September 26, 2017, 10:35:14 am
content: You need a LTspice model for the thyristor, and to include it with a .lib statement.

author: anishkgt
author_rank: Frequent Contributor
timestamp: September 26, 2017, 11:28:14 am
content: I added the symbol from LTSpice. Wouldn't the lib also present there ?Could you please direct me to any resources that i could follow to get this done.

author: Ian.M
author_rank: Super Contributor
timestamp: September 26, 2017, 12:18:02 pm
content: Didn't you read the description when you selected the SCR symbol in the component browser?It says: "Generic SCR symbol for use with a model that you supply."Search the web for a model for the SCR you want to use, which will be a .sub or .lib file (possibly zipped). .lib files can contain multiple models. A model in LTspice format is strongly preferred, as there are some syntax differences for behavioural sources that can cause problems if you attempt to use models intended for PSPICE or other SPICEs. However many PSPICE models are fully LTspice compatible. Download it and if its zipped extract it into the same folder as your simulation. Add a .lib or .inc statement to the schematic, naming the file containing the model. Use a .inc statement if its a .sub file or .lib if its a .lib file. Make sure the 'Value' field of the SCR symbol you have placed EXACTLY matches the name of the model inside the .lib or .sub file.

author: anishkgt
author_rank: Frequent Contributor
timestamp: September 26, 2017, 02:52:44 pm
content: Sorry am just beginning to learn to work with LTSpice.Still can get that error fixed. I did see it was generic but not sure how to go about it. I did not find any SCR models but just a lib file from this forum, added that file to where the schematic is saved. Is there anything that i should consider as running the simulation gives an error.How do i know if the the model matches a symbol ?here is my LTSpice net list* C:\Users\georget\Documents\LTspiceXVII\SCR_Snubber.ascXU1 N001 N003 N007 EC103D1XU2 N007 N005 N001 EC103D1C1 N006 N007 0.1µf V=400XU3 N002 0 N003 N004 NC_01 MOC205 Igain=.724mD1 N001 N003 DD2 N007 N005 DR1 N005 N004 360R2 N001 N003 360R3 N001 N006 39R4 N005 N007 360V1 N001 0 SINE(0 240 60 0 0 0 5)L1 N007 0 100µ Ipk=5L2 N009 N008 2.4µ Ipk=2000V2 N002 0 PULSE(5 5 20 1 3 3 1 0)R5 N008 N009 0.09 tol=1 pwr=200.model D D.lib C:\Users\georget\Documents\LTspiceXVII\lib\cmp\standard.dioK L1 L2 1.tran 10.lib MOC205.sub.backanno.end

author: Ian.M
author_rank: Super Contributor
timestamp: September 26, 2017, 03:19:04 pm
content: Try the attached sim. I've renamed the SCR .lib for convenience.Problems your original had:No .lib statement to provide the SCR modelU1 and U2 had an extra parameter '20A' that was invalidNo path to ground from the transformr secondary

author: anishkgt
author_rank: Frequent Contributor
timestamp: September 26, 2017, 04:14:02 pm
content: Thanks that worked like a charm.