Trying to simulate a microphone capsule, which capacitance varies sinusoidally.
LTspice rejects my syntax.
File globalrecordsRF mic.asc   uploaded to Temp

Trying to simulate a microphone capsule, which capacitance varies sinusoidally.
LTspice rejects my syntax.
File globalrecordsRF mic.asc   uploaded to Temp

I didn't mean 2*pi*cos (1k*time), I meant 2p*cos(1k*time). 2pF mulitplied by cos() .That would have resulted in a frequency of 159Hz, but at the time I didn't care.
Anyway, it doesn't work like I would like it to.
I'll try the charge formula, but what I've seen so far raises more questions than answers...

I've looked at the Help, and I'm none the wiser.
How is the formula "Cnnn n1 n2 Q=100p*x" included in the schematic?
To me it looks like a line in the netlist.
Then, should I use Q={75p+2p(cos(1*k(time)}*x ? With or wihout the parentheses?

2p is the maximum excursion from the rest value of 75p.

• One is to right-click on the capacitor's body and then type that formula, "Q=100p*x" (without the quotes), in the box where the value would go.
• Another is to right-click on just the capacitor's value, specifically on the text next to the capacitor, and type that formula in place of the capacitor's value.  When you first place a cap, its value is the placeholder "C".
• The third is to Ctrl-right-click on the capacitor's body and type the formula on the Value line, replacing the capacitor's normal value.

On Thu, Dec 5, 2024 at 06:16 AM, Jerry Lee Marcel wrote:

How is the formula "Cnnn n1 n2 Q=100p*x" included in the schematic?
To me it looks like a line in the netlist.

I take it you have never looked at the Help before. 

That is how every element is described - in Netlist form.

 

When you put a component on a schematic, and then press Run, LTspice turns it into a line of SPICE Netlist.  It includes (a) the element name, (b) the nodenames to which you connected it, and (c) its value and optional parameters.  For a capacitor, the normal value would be just a number.  For the charge model, you would use a formula such as "Q=100p*x" in place of the capacitor's value.

 

Then, should I use Q={75p+2p(cos(1*k(time)}*x ? With or wihout the parentheses?

If I remember correctly, you have to do some differentiation first, to turn voltage into charge,  or vice-versa.  For me, it is not intuitive.

 

I'm not sure that you understood what I wrote before about missing operators.  What is "2p(cos(...)"?  Is 2p a pre-defined function, or is it 2p times the cos() function? 

The same thing with k(time).  I don't think you meant for k() to be a function; I think you wanted 1k*(time),

On Thu, Dec 5, 2024 at 11:57 AM, Jerry Lee Marcel wrote:

Actually I did, many times. ...

Yes, I am quite sure you do.  I apologize.  That was my very bad attempt at some light humor.

Indeed, you're pardoned. 🙂

And many thanks, anyway.

hat is how every element is described - in Netlist form.

If you say so. Actually I use a GUI that saves me having to type a netlist.

Yes, we all do.  But this is one of the weaknesses of LTspice's Help.  All of the descriptions of each element, are stated as if we were writing netlists.

Everything there that describes each element, is described as if we were writing netlists.  It is up to us to interpret what that means.

 

If it showed graphical examples of each and every component type, it would be much longer.  I think Mike E. wanted to keep it compact.

Does it mean that, by seeing this formula, LTspice recognizes the fact that it should not expect a capacitance value, but a charge value that is interpreted differently? I see no mention of that in the Help.

Indeed, that is what happens.  Using the Charge formula with Q=<expression> is an alternate way of using capacitors.  There is no capacitance value as such, because you are specifying Charge, not Capacitance.

 

You might have missed that it states it this way: "There is also a general nonlinear capacitor available. Instead of specifying the capacitance, one writes an expression for the charge."  Note it says "Instead of specifying the capacitance" in that sentence.

 

And then the Help lists the syntax (netlist) line this way:

    Syntax: Cnnn n1 n2 Q=<expression> [ic=<value>] [m=<value>]
and there is no capacitance value on that line.

Both of those should make it clear that LTspice does not expect a capacitance value.

LTspice's Help is a mostly complete reference, but it is not the easiest to read.

I'm not sure that you understood what I wrote before about missing operators.  What is "2p(cos(...)"?  Is 2p a pre-defined function, or is it 2p times the cos() function? 

2p is two pico. I thought it would be understood tha same as k (or Meg, or G). So yes, it was meant to be a cos function of amplitude 2p Farad.

LTspice does not understand that "2p(cos(1k(time))" means 2p times cos(), nor 1k times (time).  On a blackboard we can write 2p(cos()) and the humans around us understand what we mean, but computers do not.  Computers need explicit multiply operators.  Without them, they misinterpret what we write.  By writing 2p(anything), LTspice would think that 2p() is supposed to be a function, not two values multiplied together.

 

(By the way, in your schematic yesterday, where you wrote "cos 1kt", I had incorrectly thought that the "k" was the Boltzmann constant.  I guess I came to that conclusion because it was next to "t", so my mind went in that direction.  Of course 1k will be 1000.  But it needed a "*" between the "1k" and "(time)".)

 

Andy