Defining DFLOP output

Thread Starter

Dragnovith

Joined Apr 16, 2021
16
Hello, I would like to know how do I configure the DFLOP with + -15 V or whatever other voltage. I tried several things but it still has + -1V.
DFLOP_Output.jpg
 

Attachments

dl324

Joined Mar 30, 2015
13,082
I tried several things but it still has + -1V.
As I recall, that's the default output swing for LTspice. You have to change some setting.

I can't help with that because I rarely use LTspice to simulate circuits and I never use it to simulate digital logic.
 

Papabravo

Joined Feb 24, 2006
16,773
The DFLOP has a set of parameters that are described in the LTspice Help pages.
Look under:
Circuit Elements
A. Special Functions

There is a table that lists the parameters for the digital A-devices
It includes
Vhigh The high logic level, defaults to 1
Vlow The low logic level, defaults to 0
Trise The rise time, defaults to 0
Tfall the fall time, defaults to Trise

and a couple of other parameters.

In order to set these parameters, you right click on the symbol. this brings up a dialog box for symbol attributes. right click on the Value column for the Value attribute and enter the text:

Vhigh=15V Vlow = -15V Trise=10n Tfall=10n

To use ±15V for logic levels, and 10 nano-seconds for rise and fall times.

The rise and fall times are important because the simulator can choke on discontinuous signals with infinite derivatives.
 

AnalogKid

Joined Aug 1, 2013
9,351
The flipflop has no power connections. The +/-1 V you are seeing probably is the transient protection diode networks.

Also - Standard CMOS is not rated to operate on 30 V.

Also - If the flipflop is powered with +15 V and GND, you will *seriously* overdrive the input in the negative direction with a -15 V signal.

Save us all a lot of time and just tell us -- what is it you are trying to achieve?

ak
 

Papabravo

Joined Feb 24, 2006
16,773
The flipflop has no power connections. The +/-1 V you are seeing probably is the transient protection diode networks.
Not true - it is just an arbitrary implementation choice for a functional behavioral model that can simulate lightning fast. The parameters entered on the spice "Value" line are just scaling factors. If the TS want's to experiment with high voltage logic outputs -- he can do it. It won't hurt anybody.
 

Thread Starter

Dragnovith

Joined Apr 16, 2021
16
In order to set these parameters, you right click on the symbol. this brings up a dialog box for symbol attributes. right click on the Value column for the Value attribute and enter the text:
Extremely silly question, forgive me. But when clicking with the right button, this is the dialog box that appears. I think I'm inserting it wrong, because it keeps going wrong.



1620054470073.png
 

Papabravo

Joined Feb 24, 2006
16,773
This dialog box is a list of "Attributes" and the "Value" of those attributes.

Move the cursor down to the "Value" attribute and over to the "Value" column. Right click on that box and enter the following text:

Vhigh=5 Vlow=0 Trise=10n Tfall=10n

Then Left-click on the OK button.

this will configure the dflop for +5V and 0V with rise/Fall times of 10 nanoseconds. You can of course adjust these to your particular preferences. When you return to the schematic page, go up to the menu bar and Left-Click on "View", and then, in the drop down menu, Left-Click on "Spice Netlist"

Locate the portion of the netlist where the text you entered is placed in the netlist line for the instance of that dflop.
In the netlist you will expect to see:
<InstName><SpiceModel><SpiceLIne><SpiceLine2><Value><Value2>
all strung together with intervening spaces.

Null fields are skipped. Pretty clever methodology -- don't you think?
 
Top