NAND Schmitt Trigger

[s35148]

Hi,

I'm having a problem with logic schmitt trigger.
I'm using the NAND 4093 power to 12V but in the output appear 15V, as you can see in the example attached.
Am I doing something wrong? How can I fix this?

Thanks,
S.

[OStep · Accepted solution]

You mixed-mode simulation setting is in Ideal mode, which means that the output pin drivers of digital components contain a fixed-valued ideal voltage source (5V for TTL and TIL components, and 5/10/15V depending on the suffix for CMOS components) regardless of what power sources you may have on your schematic.You have 4093_15V so it'll be driven by 15V for a logic high (and 0V for a logic low).

In Simulate->mixed-mode simulation settings, if you switch to Real mode, then the driver and receiver model behaviour is more complex; it is reasonably consistent with static behavior of the logic technology's I/O ports and the drivers and receivers are in fact powered by the voltage sources on your schematic.

In your case, you will see the output reach 10.44V and not 12V. This has to do with the interaction of the output impedance of the driver and your 1kOhm load, which is seems quite large for a logic circuit.

[s35148]

Hi Max,

I changed the "Mixed-mode simulation setting" to "Real Mode" and this circuit works fine.

But when I complicated a little bit the circuit, the simulation became so much slow and give an error.
Is there a way to fixed this?
I understand that "Real Mode" takes much time to run, but the circuit isn't nothing special.

Thanks,

S.

[OStep]

I'll need to see your circuit

[s35148]

Hi Max,

I figured out what was slowing the simulation. Was a DSWPK_4 switch that I had in the circuit, I changed to DIPSW4 and the simulation speed increased a lot. I think that changing the ground of the NOT gate also help. Is this true?
But then I found another problem, so I draw a simple schematic that shows what's happening. I have two NOTs 40106 and the output of the second stays in zero. This only happening in real simulation mode.
Is there a way to fix this?

Thanks for your help,
S.

[s35148]

Hi Max,

I found the problem again, I don't had in the circuit the power source of the NOT 40106.
Anyway, what's the best ground to use, the "ground" or the "dgnd"? I can have the two in the same circuit?

Thanks,

S.

[OStep]

Both grounds are connected to SPICE ground and therefore drive the connected net to 0Volts.

The difference is that the GROUND component sets the net name that is connected to it to '0', and you can't change that. The  DGND component comes into the schematic with a net named "GND", which could be changed to whatever desired. Also, many digital components have "GND" as the default net name that the hidden pins that power their drivers/receivers look for (applicable only in Real mode setting). For the example, here's the pins tab for 74HC_2V:

Therefore, you can just drop the the DGND component on the schematic and not have to worry about renaming net names for these digital components.

See the Mixed-Mode simulation section in the help file for a full explanation.