I am using 74LVC1G04 inverter for my circuit. The problem is I can't give a VCC value to this inverter, it showing an error like this.

WARNING: Can't resolve .param ilimit=215m*(vcc-1.1)/(5-1.1)
WARNING: Can't resolve .param ron=7.5*(5/vcc)**0.5

how to resolve this problem?

 

Hi CC,
Please post your asc file and any models so that we can try the simulation.
E

 

here it is..

 

Hi,
The circuit will not run to completion using any type of inverter IC.
How did you decide the component values and what output are you expecting.?
E

 

Hi,
The circuit will not run to completion using any type of inverter IC.
How did you decide the component values and what output are you expecting.?
E

it's a simple pierce oscillator circuit, expecting a square wave output!

 

Hi,
Could you post your component calculations, and what output frequency is expected.?
E

 

Hi,
Could you post your component calculations, and what output frequency is expected.?
E

output frequency expected around 32~ 35kHz

 

You can't use the part with an output buffer. You need to use the unbuffered part.

 

You can't use the part with an output buffer. You need to use the unbuffered part.
View attachment 294458
[/QUO
I didn't get this? can you please share this component .lib?

 

http://bordodynov.ltwiki.org/
Or click on: Additional library for LTspice, file is lib.zip ~20M
The file is large but it is in there

 

Perhaps you need a .param command to specify vcc as a parameter and to set its value.

 

I used the above inverter again the same problem.
Questionable use of curly braces in "xu2 n001 out 5v 0 74lvc1gu04 vcc={vcc} speed=1 tripdt=100p"
Error: undefined symbol in: "[vcc]"
WARNING: Can't resolve .param vcc=(vcc)
WARNING: Can't resolve .param vcc1=vcc
Questionable use of curly braces in "xin a yi vcc vgnd 74lvc_in_unbuf vcc2={vcc1}"
Error: yet unevaluated parameter in: "[vcc1]"
Questionable use of curly braces in "xout yi y vcc vgnd 74lvc_out vcc2={vcc1} speed2={speed1}"
Error: yet unevaluated parameter in: "[vcc1]"
WARNING: Can't resolve .param vcc2=(vcc1)
WARNING: Can't resolve .param vcc3=vcc2
Questionable use of curly braces in "e1 drv 0 inr vgnd table(0,1 {vcc3/2},500m {vcc3},0)"
Error: yet unevaluated parameter in: "[vcc3/]2"
Questionable use of curly braces in "e1 drv 0 inr vgnd table(0,1 (vcc3/2),500m {vcc3},0)"
Error: yet unevaluated parameter in: "[vcc3]"
WARNING: Can't resolve .param vcc2=(vcc1)
WARNING: Can't resolve .param vcc3=vcc2
WARNING: Can't resolve .param ilimit=215m*(vcc-1.1)/(5-1.1)
WARNING: Can't resolve .param ron=7.5*(5/vcc)**0.5

 

I used the above inverter again the same problem.
Questionable use of curly braces in "xu2 n001 out 5v 0 74lvc1gu04 vcc={vcc} speed=1 tripdt=100p"
Error: undefined symbol in: "[vcc]"
WARNING: Can't resolve .param vcc=(vcc)
WARNING: Can't resolve .param vcc1=vcc
Questionable use of curly braces in "xin a yi vcc vgnd 74lvc_in_unbuf vcc2={vcc1}"
Error: yet unevaluated parameter in: "[vcc1]"
Questionable use of curly braces in "xout yi y vcc vgnd 74lvc_out vcc2={vcc1} speed2={speed1}"
Error: yet unevaluated parameter in: "[vcc1]"
WARNING: Can't resolve .param vcc2=(vcc1)
WARNING: Can't resolve .param vcc3=vcc2
Questionable use of curly braces in "e1 drv 0 inr vgnd table(0,1 {vcc3/2},500m {vcc3},0)"
Error: yet unevaluated parameter in: "[vcc3/]2"
Questionable use of curly braces in "e1 drv 0 inr vgnd table(0,1 (vcc3/2),500m {vcc3},0)"
Error: yet unevaluated parameter in: "[vcc3]"
WARNING: Can't resolve .param vcc2=(vcc1)
WARNING: Can't resolve .param vcc3=vcc2
WARNING: Can't resolve .param ilimit=215m*(vcc-1.1)/(5-1.1)
WARNING: Can't resolve .param ron=7.5*(5/vcc)**0.5

Do it like this:

 

Do it like this:
View attachment 294483

Thank you so much! The circuit is working fine now.. So I have a question, what is happening between giving a Vcc pin like this in the above figure and by using a label or VCC from the component?

 

Thank you so much! The circuit is working fine now.. So I have a question, what is happening between giving a Vcc pin like this in the above figure and by using a label or VCC from the component?

The explanation requires that you become familiar with the SPICE netlist generated by LTspice from your schematic. This SPICE netlist is regenerated on the fly in the simulator and is not generally saved. You can view the netlist in a dialog box by selecting from the menu bar:
View | SPICE Netlist

* C:\Users\%HOMEPATH%\Documents\LTspiceXVII\examples\Temp\0-9\Draft4.asc
XU1 in out N001 0 74LVC1GU04 VCC={VCC} Speed=1 Tripdt=100p
V1 in 0 PULSE(0 5 0 50n 50n 500u 1m)
V2 N001 0 {VCC}
.tran 5m
.param VCC=5V
.lib 74LVC1G.lib
.backanno
.end

Notice the form of the assignment invoking the subcircuit. The external node {VCC} is being assigned to the internal name VCC in the subcircuit. It is done this way for several reasons. One is that the power and ground connections are not necessarily required. Some people like them so they can measure device currents.

If you open up the symbol in the Symbol Editor you will notice that the symbol has the required parameters in the SpiceLine field.


There are certainly other ways to do things, but as one of my mad friends is fond of observing:

"There is something about every system that sucks."​

 

The explanation requires that you become familiar with the SPICE netlist generated by LTspice from your schematic. This SPICE netlist is regenerated on the fly in the simulator and is not generally saved. You can view the netlist in a dialog box by selecting from the menu bar:
View | SPICE Netlist

* C:\Users\%HOMEPATH%\Documents\LTspiceXVII\examples\Temp\0-9\Draft4.asc
XU1 in out N001 0 74LVC1GU04 VCC={VCC} Speed=1 Tripdt=100p
V1 in 0 PULSE(0 5 0 50n 50n 500u 1m)
V2 N001 0 {VCC}
.tran 5m
.param VCC=5V
.lib 74LVC1G.lib
.backanno
.end

Notice the form of the assignment invoking the subcircuit. The external node {VCC} is being assigned to the internal name VCC in the subcircuit. It is done this way for several reasons. One is that the power and ground connections are not necessarily required. Some people like them so they can measure device currents.

If you open up the symbol in the Symbol Editor you will notice that the symbol has the required parameters in the SpiceLine field.
View attachment 294489

There are certainly other ways to do things, but as one of my mad friends is fond of observing:

"There is something about every system that sucks."​

Thank you so much for this info! Greatly appreciated your help!

 

Do it like this:
View attachment 294483

Hi, If I want to add one more IC (from your doc. ie;74LVC1G17_IEEE \lib\sym\ZZZ\LOGIC\74LVC1G_alt\IEEE)at the output of 74LVC1GU04, how can I add? I am getting an unknown sub circuit error while adding this. I added lib file in the directive (.lib 74LVC1G1_alt.lib) but still error...

 

Hi, If I want to add one more IC (from your doc. ie;74LVC1G17_IEEE \lib\sym\ZZZ\LOGIC\74LVC1G_alt\IEEE)at the output of 74LVC1GU04, how can I add? I am getting an unknown sub circuit error while adding this. I added lib file in the directive (.lib 74LVC1G1_alt.lib) but still error...

Place your 74LVC1G17 symbol on a schematic. Right-click on the symbol to open the "Component Attribute Editor" dialog box. In the upper left corner, there is an "Open Symbol" button.

This will open the Symbol Editor. Nows use the Ctrl-A (That's the Control key and the letter A) to open the "Symbol Attribute Editor"

Look at the "ModelFile" attribute to see if it points to the correct library "74LVC1G.lib". Then open up the library in a text editor and verify the model is included.

Notice there are revisions to the library and your copy might be out of date. The most up-to-date versionis the one from the LTspice user's group on groups.io

 

Place your 74LVC1G17 symbol on a schematic. Right-click on the symbol to open the "Component Attribute Editor" dialog box. In the upper left corner, there is an "Open Symbol" button.
View attachment 294948
This will open the Symbol Editor. Nows use the Ctrl-A (That's the Control key and the letter A) to open the "Symbol Attribute Editor"
View attachment 294943
Look at the "ModelFile" attribute to see if it points to the correct library "74LVC1G.lib". Then open up the library in a text editor and verify the model is included.
View attachment 294945
Notice there are revisions to the library and your copy might be out of date. The most up-to-date version is the one from the LTspice user's group on groups.io

Yes, You are right! my library copy is out of date! I am new to groups.io group, where can I find the up to date version of the library files?
Thank you so much for the help!

 

Do it like this:

I believe it will also work if you label the V2 output node Vcc.