[Bug-gnucap] Re: [Help-gnucap] Flip-flop RS

[Jose Roberto B. de A. Monteiro]

Hello Al,

al davis wrote:
> The digital portion has not been well tested recently.  The 
> regression suite has only very sparse coverage.  Although I 
> think it worked years ago, this part has really only 
> had "student PhD project" level testing.  Part of what you 
> report is bugs, with an easy fix.  Part is "correct" behavior.
>
> On Friday 04 August 2006 08:29, Jose Roberto B. de A. Monteiro 
> wrote:
>
>   
>> The DC simulation gave the result as follows:
>> #           V(V2)      V(V3)      V(U1)      V(U2)
>>   0.         0.         10.        5.         0.
>>   2.         2.         10.        5.         0.
>>   4.         4.         10.        5.         0.
>>   6.         6.         10.        5.         0.
>>   8.         8.         10.        5.         0.
>>   10.        10.        10.        5.         0.
>>
>> Now the output have a numeric answer but is not as expected.
>> If it is a CMOS type logic, the expected answer for V(U1) is
>> 10V, like V1. 
>>     
>
> This part is actually working as designed.  In digital mode, the 
> value at a node is a logic state, not a voltage.  If you 
> probe "logic(U1)" it will tell you the logic state which is 
> coded as "3." which means "stable 1".
>
> The voltage is generated by a conversion based on the parameters 
> in the .model statement.  In particular "vmax".  Since you 
> didn't say, it is 5 volts.
>   
Ok... I understand... but, IMHO the digital simulator would be
wonderfully flexible if it took its high voltage output level from its
VCC pin, and it LOW voltage output level from its GND pin. Otherwise,
since its uses a "hardcoded" output voltage, VCC and GND pins are
useless, for output, at least. How does it determine input levels? From
VCC and GND pins potential?

The use of VCC and GND pins voltage potentials would be useful in
applications were logics are connected in different GNDs and VCCs. It is
the case for some analog/digital mixed circuits, as in cmos analog
switches for data aquisition systems (analog channel multiplexes).

The same thing I believe would be usefull for tanh function. Let me
explain: I use a VCVS for modeling a opamp. for example: E1 3 0 1 2 tanh
gain=10MEG limit=12. This line simulates a opamp (very simple) with an
open gain of 10e6 and fed by +12V and -12V. (I thoght about other
possible opamps, but it seems to be the most light, unless you know a
better one.) The inverted input is note 2, non-inv. is node 1, output at
node 3 and gnd at 0, of course. If it would be possible to write: E1 3 0
1 2 tanh gain=10MEG upperlimit=V(VCC) lowerlimit=V(VEE) it would be
great! It would be possible to make a subcircuit for an opamp very
simple, and, I belive, very light is terms of data processing:

.subckt opamp OUT GND VCC VEE NINV INV
E1 OUT GND GAIN=10MEG upperlimit=V(VCC) lowerlimit=V(VEE)
.ends

And could use this opamp as a symbol calling this subcircuit in my
schematic:

X1 3 V0 V1 V2 1 2 opamp
>   
>> And, if V2 is 10V in the last line, V(U1) and 
>> V(U2) should be both equal to 0.
>>     
>
> This one is a bug.  If you look at the logic value, you would 
> see that it changes to state 2, which is "falling", which means 
> it is currently a 1, but a change to 0 is pending.  
>
> The bug is that the actual change never happens.  I think this 
> one was introduced a long time ago as a result of some other 
> rework, but I am not sure just what or why.  It might have 
> happened when code was converted from C to C++.
>
> I didn't see it, because I have been doing mostly pure analog 
> since then, and when used in true mixed-mode, it is common to 
> have both analog and digital models of such a device.  The 
> simulator would notice the issue with the digital only side, 
> and use the analog model to determine what is really correct.  
> In this particular circuit, you run 5 volt logic on 10 volts, 
> which alone is enough to tell the simulator to use the analog 
> model if it has one.
>
> The fix is simple.  I will post it after a little more testing.
>
>   
>> I tried a simple simulation for a transient analisys but I've
>> got a seg fault! The script is the following (the circuit is
>> the same):
>>     
>
> This one is a bug introduced recently as part of some efficiency 
> improvements.  The "subckt" attachment was changed from an 
> object to a pointer.  What was an empty subckt is now a null 
> pointer, which needs to be checked.  Just checking for a null, 
> and skipping the action if it is null, fixes the 
> problem.  "dc_begin" has the correct code.  "tr_begin" doesn't.  
> I will post it after a little more testing.
>
> You can ignore the messages:
> can't find subckt: CMOSnor2
> U2: no model, forcing digital
>
> They just tell you that since there is no analog model it is 
> always using the digital model.
>
>   
>> Someone else tried to use a TTL subcircuit for the NOR gates,
>> but he got a segfault too.
>>     
>
> If there really is a subcircuit, he should not get the segfault.  
> Just changing CMOS to TTL really doesn't change anything.  
> Those names are just strings to the simulator, with no special 
> meaning.
>
>
>
> The next development snapshot will have documentation updates, 
> Muntzing, and minor updates called for by formal testing.  No 
> feature changes.
>
>
>