...umm, Helmut...are they gonna call this LTSPICE 17? or LTSPICE 5?

Or Mike E.'s? strawberry wonder pudding?

<---is bad at attempts at Brit* humour.

Oh and by the way Helmut, tell mr Mike...I noticed something weird (workable perhaps)..but still

""unusual"".

When activating the 64-bit version of LTSPICEXVIII...using WINE loader (not Qt WINE) 1.7 in Fedora 21

FEL (Fedora Electronics Lab)...I briefly get a "black box window" (instead of the usual WINE box).

Might be a graphics memory management issue....the program still ran properly (I have not tested the

32-bit version of LTSPICEXVIII)...hmmm.

Could indicate "issues down the road" mr. Mike (all the related graphics worked as well including FFT

transforms and inverse-transforms(.

W. Warren

*(hopes John can think of something better...just a homeboy here in Fort Worth Texas)

Wow!



Thanks for the new version including TVS Diodes.



I think I saw a problem with one of the models. I have given some information to see if you duplicate my test. Maybe I am doing something wrong.





The SMCJ33A Model seems to have issues with low clamp currents.







Set up the following scenario:



Test Circuit

Circuit is Voltage Source

Series Current Limiting Resistor

Parallel TVS after the Series Current Limit Resistor

Ground





Make a pulse source

Starting voltage = 28V

Vmax = 80V

Delay =10ms

Rise & fall times = 1us

Time on = 50ms

Period = 100ms



Series Resistor Initial Value = 100m



TVS = SMCJ33A



Simulation set-up

Stop time = 200m

Time Step = 0.1us

Don’t open the simulation with DC at 0V.





Run the simulation with the 100m Ohm Series Resistor

Probe the source voltage on the left side of the series limiting resistor.

Probe the TVS Voltage at the right side of the series limiting resistor.



Clamped Waveform looks marginally correct.

Observation of source waveform:

The waveform starts at 28V, rises to 80V Pulse, returns to 28V, starts identical cycle. Correct



Observation of TVS waveform:

The waveform starts at 28V, rises to 64V Pulse, returns to 28V, starts identical cycle. The waveform fall below 24V (the <24V is not correct).





Change the 100m resistor to 100 Ohms.







Run the simulation again with the 100 Ohm Resistor



Clamped Waveform looks is wrong

Observation of source waveform:

The waveform starts at 0V, rises to 80V Pulse, returns to 28V, starts identical cycle. Correct



Observation of TVS waveform:

The waveform starts at 0.93V, rises to 1.064V Pulse, returns to 0.93V, starts identical cycle. The waveform should loosely follow the previous TVS Waveform above. It doesn’t and appears to be a representation of the clamped current within the TVS device (which is also incorrect – there should be no current flowing through the device). If a 10k Load is placed across the TVS is still does the same thing.









The SMBJ24CA doesn’t have the same behavior. It seems to be much better behaved. Change the Starting Voltage to 15V for that simulation.





Can you check it out – it looks like there is a problem with the SMCJ33A TVS Model.



Thanks,



Ross







From: LTspice@... [mailto:LTspice@...]
Sent: Thursday, July 28, 2016 6:09 PM
To: [LTspice] group
Subject: Re: [LTspice] Re: LTspiceXVII released





"are they gonna call this LTSPICE 17 or LTSPICE 5?"



It seems that they (LTC) or he (Mike) have given it the name LTspice XVII. This program is released. The name is what it is.



By the way, you might want to pay closer attention to the capitalization. Some people get upset when it is done wrong. Neither Mike nor LTC uses "LTSPICE". Also, only two I's in XVII.



"Oh and by the way Helmut, tell mr Mike...I noticed something weird ..."



You should tell him yourself; don't make Helmut do the work for you. Mike shows how to report bugs and other problems. See Help -> About LTspice XVII. (But I am not sure if this one is an LTspice issue or a Wine issue.)



"...just a homeboy here in Fort Worth Texas"



Very much O.T. now -- but I wonder why you posted that link earlier today to a UML (Massachusetts) webpage which didn't have any obvious links to the T.I. patent issue you were describing. Fort Worth and Lowell are very much not local to one another. It just had my curiosity. No big deal.



Andy









[Non-text portions of this message have been removed]

开云体育

The state machine appears to have a bug.? The nominal output amplitude is 1mV rather than 1V, so the output equations must be multiplied by 1k.? For example:

.output (2) (V(1)<.5)*1k
.output (3) (V(1)>.5)*1k
.output (4) state*1k

Also (not bugs):

The .output are voltage sources, but are considered to be floating, thus they must be loaded with a resistor or other device that provides a path to ground.

The triptdt parameter only affects output edges that are triggered by state changes, not output edges that are dependent only on inputs.

Hello Vlad

See the help with keyword "state"? [ .MACHINE -- Arbitrary State Machine ] in LTspice XVII

Regards
PhB

Hello analogspiceman,

开云体育

Hello Helmut,

Try the second example from Help (just paste it into an empty schematic as SPICE text).? It is true that the outputs will sum together like current sources, but the value of the load resistors has no effect on the output amplitude.? Please try it and report back.

Hello analogspiceman,

Hello Helmut,

Just to be sure I just reinstalled the new LTspice from their website.? I am running Windows 7 Home Premium 64 bit I-7.

Hello analogspiceman,

Hello Helmut,

V1 1 0 pulse(0 1 0 1u 1u .5m 1m)
R1 2 0 1.5k
*R2 2 0 1g
.machine
.output (2) V(1) < .5
.endmachine
.tran 3m

If I run the above netlist, it only produces 1mV on node 2, but the error log shows why:

WARNING: Less than two connections to node 1.? This node is used by V1.
WARNING: Less than two connections to node 2 of instance R1:? Node and device optimized out.

If I un-comment R2, then it produces 1.5V on node 2.? This is unexpected.? Using the netlist exactly as shown in the Help file does not produce 1V as expected (at least for me).

Your netlist shown below works as expected.

Hello Helmut,

I now understand the cause of the strange behavior.? I had "Enable beta circuit matrix operations" checked in the Hacks! tab of the Control Panel.? Apparently, among that option's various functions, it removes single component circuit islands.

What is interesting is that my selection of this option managed to persist through a complete reinstall of the software.? The Control Panel's persistent settings must be stored in the registry or in a configuration file that does not get erased or overwritten.? I will have to go looking for where such items are stored with the new LTspice.