csd17506q5a spice model - Page 1
Forum section: electronics / general

author: SpeedrunnerG55
author_rank: Newbie
timestamp: October 06, 2022, 07:24:16 pm
content: I don't know much about getting transistor models into spice.But I downloaded the spice model for the CSD17506Q5A n channel power MOSFET from the Texas Instruments website.I tried to use it but it does not work.it seems to me there are more steps involved that are not apparent when I look up tutorials> Compatibility modes selected: ps lt> warning, can't find model 'csd17506q5a' from line> q2 net-_d2-pad2_ net-_d2-pad2_ net-_d2-pad2_ net-_l4-pad2_ /cap csd17506q5a> warning, can't find model 'csd17506q5a' from line> q4 gnd gnd gnd net-_b1-pad1_ net-_d2-pad2_ csd17506q5a> warning, can't find model 'csd17506q5a' from line> q3 gnd gnd gnd net-_b2-pad1_ net-_d1-pad2_ csd17506q5a> warning, can't find model 'csd17506q5a' from line> q1 net-_d1-pad2_ net-_d1-pad2_ net-_d1-pad2_ net-_l1-pad2_ /cap csd17506q5a> Circuit: KiCad schematic> Error on line 5 :> q2 net-_d2-pad2_ net-_d2-pad2_ net-_d2-pad2_ net-_l4-pad2_ /cap csd17506q5a> could not find a valid modelname> Background thread stopped with timeout = 0> Error: circuit not parsed.any ideas?

author: Benta
author_rank: Super Contributor
timestamp: October 06, 2022, 11:57:18 pm
content: Too little information.Just downloading is not enough, the model needs to integrated in your schematic's device. Tell us what you've done.As you're posting in the KiCAD section, I expect we're talking ngspice?

author: SpeedrunnerG55
author_rank: Newbie
timestamp: October 07, 2022, 12:44:43 am
content: Yes ngspiceI selected the lib file for each of the symbols.I just noticed the model was set to BJT... not sure why. changed that to subcircuit.changed the alternate node sequence to 5 4 1but now it's giving me different messagesCode:Compatibility modes selected: ps ltCircuit: KiCad schematicOriginal line no.: 0, new internal line no.: 116:Undefined number Original line no.: 0, new internal line no.: 116:Cannot compute substituteOriginal line no.: 0, new internal line no.: 122:Undefined number Original line no.: 0, new internal line no.: 122:Cannot compute substituteOriginal line no.: 0, new internal line no.: 148:Undefined number Original line no.: 0, new internal line no.: 148:Cannot compute substituteOriginal line no.: 0, new internal line no.: 116:Undefined number Original line no.: 0, new internal line no.: 116:Cannot compute substituteOriginal line no.: 0, new internal line no.: 122:Undefined number Original line no.: 0, new internal line no.: 122:Cannot compute substituteOriginal line no.: 0, new internal line no.: 148:Undefined number Original line no.: 0, new internal line no.: 148:Cannot compute substituteOriginal line no.: 0, new internal line no.: 116:Undefined number Original line no.: 0, new internal line no.: 116:Cannot compute substituteOriginal line no.: 0, new internal line no.: 122:Undefined number Original line no.: 0, new internal line no.: 122:Cannot compute substituteOriginal line no.: 0, new internal line no.: 148:Undefined number Original line no.: 0, new internal line no.: 148:Cannot compute substituteOriginal line no.: 0, new internal line no.: 116:Undefined number Original line no.: 0, new internal line no.: 116:Cannot compute substituteOriginal line no.: 0, new internal line no.: 122:Undefined number Original line no.: 0, new internal line no.: 122:Cannot compute substituteOriginal line no.: 0, new internal line no.: 148:Undefined number Original line no.: 0, new internal line no.: 148:Cannot compute substituteCopies=91 Evals=416 Placeholders=13 Symbols=28 Errors=24Numparam expansion errors: Problem with input file.Error: ngspice.dll cannot recover and awaits to be detachedNote: can't find init file.******** ngspice-36 shared library** Creation Date: Sat Jan 1 18:54:42 UTC 2022******Error: there aren't any circuits loaded.

author: hvogt
author_rank: Contributor
timestamp: November 06, 2022, 08:07:38 am
content: Unfortunately the model in csd17506q5a.lib has syntax incompatible to ngspice (and the PSPICE manual). If you change it (lines 43 ff) like:Code:.PARAM ptrc1 = 5.5e-3.PARAM ptrc2 = 10.0e-6.PARAM pwidthP = 1.972.PARAM pwidth = {pwidthP*1e6}.PARAM perimP = {2.1*pwidthP}.PARAM perim = {perimP*1e6}(see the '=' token), it will be o.k.. Even better if you addCode:.option gmin=1e-11to your netlist, e.g. as a text box on the Eeschema canvas.