new spice models available

[andrei]

No, axis are fit by straight lines now...

 

[Majestic]

Hi,

Don't want to hijack this thread, but didn't want to start a new one specifically just for my question either...

But, I'm trying to teach myself the ins and outs of SPICE modeling right now, are there any reccomended introductory texts to the program at all?

Also, what SPICE variant do fellow DIY-ers reccomend and use at the moment? Given that there seem to be a few to choose from, is there a clear winner in this area right now??

 

[kevinkr]

I like and use LTspice for the following reasons. I recommend it highly.

Unlimited node and component count.

Lots of tube and other device models that will run in LTspice, AFAIK all 3F4 models will run without changes.

It's free.

It's not too hard to use with a graphical interface for drawing schematics that is reasonably user friendly.

It is somewhat complicated getting models into LTspice, has to be done via the OS. (Add model to sub(ckt) directory, symbol to appropriate subdirectory under sym (symbol)

Need to know very little about spice, help is extensive and useful.

Usual problems are simulations don't converge in the default number of iterations (typically dc op point) and you have to add a statement to the schematic to increase the iterations. (This is true in all versions of spice I have tried.)

I previously used MCAP8 student and professional editions, however the student version is limited to 50 nodes and 100 components. The full version is expensive.

 

[pedroskova]

I just model the PSU in PSUDII and the signal circuits in MCAP8. Like Kevin pointed out, the "student" edition is limited, but it has been able to handle most everything this rookie has tried, and is very easy to use.

 

[andrei]

I like Spice OPUS.

 

[audiobot]

subckt where?

Being an idiot adrift in the world of spice, could someone write out exactly what and where I put a tube model into LTSpice so that the engine will recognize it?

I tried entering this as a Spice Directive

.subckt 5687 curves markers P G K
Bp P K I=(0.1305431537m)*uramp(V(P,K)*ln(1.0+(-0.02783234437)+exp((6.358374034)+(6.358374034)*((18.10314636)+(-49.38307311m)*V(G,K))*V(G,K)/sqrt((23.05269276)**2+(V(P,K)-(-0.7195968334))**2)))/(6.358374034))**(1.26765549)
.ends

and putting

5687 curves markers

into the value line of the tube in the schematic, but it won't accept this or any other variation I have tried.

Thanks for any help,

Michael

 

[andrei]

Model name should not have spaces in it... So do something like (either as a Spice directive or in .included file):

.subckt 6SN7 P G K
Cgp G P 4.0p
Ci G K 2.6p
Co P K 0.7p
Bp P K I=(0.02101361337m)*uramp(V(P,K)*ln(1.0+(-0.07065996889)+exp((4.906641927)+(4.906641927)*((21.00937615)+(-88.11984935m)*V(G,K))*V(G,K)/sqrt((26.83919821)**2+(V(P,K)-(5.377562838))**2)))/(4.906641927))**(1.370968473)
.ends 6SN7

Then set model parameters as in the attached screen shot.

 

[audiobot]

Most excellent

Andrei,

Thank you, that did the trick. I haven't played with spice in a year or so and I wasn't competent then. I do distinctly remember having similar problems then, but I have changed computers and I couldn't find any old files to refer to.

Your curve captor seems to work well, once I sort have figured out how to enter the values. Still some work to do on that front too.

Thanks again,
Michael

 

[audiobot]

Another question

Does the model generated by curve captor account for C g-p? Or do I have to put a bogey cap into the spice simulation? My hf behaviour is not quite right I think.

Thanks,

Michael

 

[Joel]

Does the model generated by curve captor account for C g-p?

No.

 

[mod_evil]

Does anybody know how I put Pentode models in CircuitMaker Student version? I need to simulate a amplifier with EL84, 6v6 and EL34...

Thanks a lot of!

 

[aletheian]

Does anybody know how I put Pentode models in CircuitMaker Student version? I need to simulate a amplifier with EL84, 6v6 and EL34...

Thanks a lot of!

Just use the tetrode model and put in your pentode parameters. That will assume that the surpressor is tied to ground

 

[jackinnj]

Hi Joel,
Any possibility of you doing models for 45, 50 2A3, 300B, 211, 845..
The 2A3 and 300 B models I have ported to LTspice take forever to converge if they do at all.

I haven't bothered to input the correct inter-electrode capacitances, so you'll have to get them off the data sheet.

.subckt 45TUBE 1 2 3
+Params: MU=3.711 KP=36.03 KVB=100 EX=1.376 KG1=4379
E1 7 0 Value = {(V(1,3)/KP)*LN((1+ EXP((KP/MU) + ((KP*(V(2,3)))/(SQRT(KVB+V(1,3)*V(1,3)))))))}
RE1 7 0 1e12
G1 1 3 VALUE = {(((V(7))^EX)/KG1)*(1+SGN(V(7)))}
RCP 1 3 1e12
C1 2 3 2.4e-12
C2 1 2 3.9e-12
C3 1 3 0.7e-12
R1 2 5 1000
D3 5 3 dx
.model dx d(is=1e-09 rs=1 cjo=10e-12)
.ends

An externally hosted image should be here but it was not working when we last tested it.

.subckt 45TUBE 1 2 3
+Params: MU=3.943 KP=58.17 KVB=2050 EX=1.50 KG1=1517
E1 7 0 Value = {(V(1,3)/KP)*LN((1+ EXP((KP/MU) + ((KP*(V(2,3)))/(SQRT(KVB+V(1,3)*V(1,3)))))))}
RE1 7 0 1e12
G1 1 3 VALUE = {(((V(7))^EX)/KG1)*(1+SGN(V(7)))}
RCP 1 3 1e12
C1 2 3 2.4e-12
C2 1 2 3.9e-12
C3 1 3 0.7e-12
R1 2 5 1000
D3 5 3 dx
.model dx d(is=1e-09 rs=1 cjo=10e-12)
.ends

An externally hosted image should be here but it was not working when we last tested it.

EDIT -- I plugged them into multi-sim and they seem to work very well.