Voltage-variable capacitor doesn't work in LTSpice

On Wed, 18 Mar 2015 07:09:56 -0700, Joerg <news@analogconsultants.com>
wrote:

[snip]
Guys, I do not want to change the capacitance by changing the voltage at
the cap terminals. I want to change the capacitance by a mathematical
expression where the control function is a rail (or a voltage) in some
other distant land in the schematic. I still do not understand why this
works perfectly for a resistor value but it does not for a capacitor
value. For the resistor I do not have to make some other model with more
terminals, I can just key in expressions such as "R=V(X)" in the value
field where X is a rail somewhere else that I assign the label "X".

My previously posted subcircuit VControlledCap does exactly as you
want.

I have just now posted VControlledCap.asy so you can get the pinout
correct >:-}

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Voltage-Controlled Capacitor Spice Model now on my website.

See VControlledCap.zip on the Device Models & Subcircuits Page.

Includes Library File (.LIB), LTspice Symbol (.ASY), and a JPEG
showing how it was developed.

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Den onsdag den 18. marts 2015 kl. 21.36.27 UTC+1 skrev Joerg:
On 2015-03-18 11:54 AM, Syd Rumpo wrote:
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.


Tried it and that completely bungled the linearity when the cap is
inside a resonant circuit. At least no more error messages which is
good. Well, maybe I just do it in hardware then, firing up the old
Weller. I'd have to buy a bag of varicaps but those are cheap.

http://powerelectronics.com/site-files/powerelectronics.com/files/archive/powerelectronics.com/mag/504PET07.pdf

-Lasse
 
On Wed, 18 Mar 2015 09:28:57 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

Voltage-Controlled Capacitor Spice Model now on my website.

See VControlledCap.zip on the Device Models & Subcircuits Page.

Includes Library File (.LIB), LTspice Symbol (.ASY), and a JPEG
showing how it was developed.

...Jim Thompson

I don't have time to play with this just now, but one quick question:

Given that C is a variable capacitor, set C to 1F and charge it to 1
volt. Now change C to 0.5F. What is the new voltage?


--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
On Wed, 18 Mar 2015 17:40:06 +0000 (UTC), DecadentLinuxUserNumeroUno
<DLU1@DecadentLinuxUser.org> wrote:

On Wed, 18 Mar 2015 10:30:44 -0700, John Larkin wrote:

On Wed, 18 Mar 2015 09:28:57 -0700, Jim Thompson
To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

Voltage-Controlled Capacitor Spice Model now on my website.

See VControlledCap.zip on the Device Models & Subcircuits Page.

Includes Library File (.LIB), LTspice Symbol (.ASY), and a JPEG showing
how it was developed.

...Jim Thompson

I don't have time to play with this just now, but one quick question:

Given that C is a variable capacitor, set C to 1F and charge it to 1
volt. Now change C to 0.5F. What is the new voltage?

How many 1 farad capacitors are you aware of?

In LT Spice, you can use any C value. 1F is the generic capacitor. I
usually normalize theoretical circuits to 1F, 1H, 1 ohm. [1]

In real life, Digikey will sell you 1F caps. Or 5000F caps. But not
variable 1F caps.

Oh and would not a 1F charged cap dump into a 0.5F cap and fully charge
it? If that answer is yes, then the voltage would be the same...
slightly less even, all elements considered.

You thought it would morph the EMF into something else?

I'd like to know if Jim's model conserves charge, or conserves energy,
or conserves voltage. Or whatever it does.


[1] I do find myself picking standard values, like 39nF instead of 40
nF, and worrying about leakage and stray capacitance and power
dissipation, when none of these matter in Spice.



--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
On Wed, 18 Mar 2015 10:30:44 -0700, John Larkin
<jlarkin@highlandtechnology.com> wrote:

On Wed, 18 Mar 2015 09:28:57 -0700, Jim Thompson
To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

Voltage-Controlled Capacitor Spice Model now on my website.

See VControlledCap.zip on the Device Models & Subcircuits Page.

Includes Library File (.LIB), LTspice Symbol (.ASY), and a JPEG
showing how it was developed.

...Jim Thompson

I don't have time to play with this just now, but one quick question:

Given that C is a variable capacitor, set C to 1F and charge it to 1
volt. Now change C to 0.5F. What is the new voltage?

I haven't tried that. Since it _is_ a capacitor, it'll depend on
whether a simulator treats capacitors as charge-controlled devices or
otherwise.

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Voltage-Controlled Resistor Spice Model Updated

See VVR.zip on the Device Models & Subcircuits Page of my website

Includes Library File (.LIB), LTspice Symbol (.ASY), PSpice Symbol
(.SYM)and a JPEG showing how it was developed.

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.

Cheers
--
Syd
 
On Wednesday, March 18, 2015 at 1:54:56 PM UTC-4, John Larkin wrote:
On Wed, 18 Mar 2015 17:40:06 +0000 (UTC), DecadentLinuxUserNumeroUno
DLU1@DecadentLinuxUser.org> wrote:

On Wed, 18 Mar 2015 10:30:44 -0700, John Larkin wrote:

On Wed, 18 Mar 2015 09:28:57 -0700, Jim Thompson
To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

Voltage-Controlled Capacitor Spice Model now on my website.

See VControlledCap.zip on the Device Models & Subcircuits Page.

Includes Library File (.LIB), LTspice Symbol (.ASY), and a JPEG showing
how it was developed.

...Jim Thompson

I don't have time to play with this just now, but one quick question:

Given that C is a variable capacitor, set C to 1F and charge it to 1
volt. Now change C to 0.5F. What is the new voltage?

How many 1 farad capacitors are you aware of?


In LT Spice, you can use any C value. 1F is the generic capacitor. I
usually normalize theoretical circuits to 1F, 1H, 1 ohm. [1]

In real life, Digikey will sell you 1F caps. Or 5000F caps. But not
variable 1F caps.


Oh and would not a 1F charged cap dump into a 0.5F cap and fully charge
it? If that answer is yes, then the voltage would be the same...
slightly less even, all elements considered.

You thought it would morph the EMF into something else?

I'd like to know if Jim's model conserves charge, or conserves energy,
or conserves voltage. Or whatever it does.
Well, energy conservation seems silly... if you are changing C,
moving plates around, someone has to provide the energy.
And I assume charge or voltage depends on how it's hooked up.

George H.
[1] I do find myself picking standard values, like 39nF instead of 40
nF, and worrying about leakage and stray capacitance and power
dissipation, when none of these matter in Spice.



--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
Den torsdag den 19. marts 2015 kl. 00.34.08 UTC+1 skrev Joerg:
On 2015-03-18 2:50 PM, Jim Thompson wrote:
On Wed, 18 Mar 2015 14:44:39 -0700, Joerg <news@analogconsultants.com
wrote:

On 2015-03-18 2:15 PM, Jim Thompson wrote:
On Wed, 18 Mar 2015 14:03:07 -0700, Joerg <news@analogconsultants.com
wrote:

[snip]


No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.


[snip]

I take it you haven't tried my subcircuit?


I have not given up yet but so far I got all kinds of error messages.
The next step would be to try it on an XP machine where I'd have to get
LTSpice going again. XP was IMHO the last known good OS and I've had
error message in other software caused by Windows 7 (meaning they didn't
happen on an XP machine).

What kind of error messages?

If you use the LTspice _symbol_ I made, you need to open the .ASY file
with a text editor and change the path to wherever you've located the
subcircuit definition library.


And there is the first problem. Windows 7 no longer allows writes to the
program directories. Well, it does but secretly stashes them some place
else but then access become an issue. I'll get to the ground of that,
hav to for my CAD as well, just not right now. The usual, swamped in
work plus honey-do stuff.

tried right-click "run as administrator" ?

you can put stuff the program directory you just have to copy and say yes to a UAC prompt


-Lasse
 
On 2015-03-18 11:54 AM, Syd Rumpo wrote:
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.

Tried it and that completely bungled the linearity when the cap is
inside a resonant circuit. At least no more error messages which is
good. Well, maybe I just do it in hardware then, firing up the old
Weller. I'd have to buy a bag of varicaps but those are cheap.

--
Regards, Joerg

http://www.analogconsultants.com/
 
On Wed, 18 Mar 2015 13:36:27 -0700, Joerg <news@analogconsultants.com>
wrote:

On 2015-03-18 11:54 AM, Syd Rumpo wrote:
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.


Tried it and that completely bungled the linearity when the cap is
inside a resonant circuit. At least no more error messages which is
good. Well, maybe I just do it in hardware then, firing up the old
Weller. I'd have to buy a bag of varicaps but those are cheap.

Are you trying to sim a VCO? Simulating oscillators is always tedious.

You could use a diode model, which does include variable capacitance.

https://dl.dropboxusercontent.com/u/53724080/Circuits/Caps/Cap_Sweep.asc

Try to get the Skyworks sample kit. It has a lot of varicaps, and many
other cool things.



--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
On Wed, 18 Mar 2015 18:54:11 +0000, Syd Rumpo <usenet@nononono.co.uk>
wrote:

On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.

Cheers

Q is charge and X is the cap voltage.

Q = (expression) * X

just means that (expression) is the capacitance. Seems silly to me.

http://ltwiki.org/LTspiceHelp/LTspiceHelp/C_Capacitor.htm

I tried a capacitor that changes value abruptly at 0 volts, like the
example. That works. If I try to change C abruptly at a non-zero
voltage, the sim crashes. Some conservation thingie was violated.




--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
On 2015-03-18 1:46 PM, John Larkin wrote:
On Wed, 18 Mar 2015 13:36:27 -0700, Joerg <news@analogconsultants.com
wrote:

On 2015-03-18 11:54 AM, Syd Rumpo wrote:
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.


Tried it and that completely bungled the linearity when the cap is
inside a resonant circuit. At least no more error messages which is
good. Well, maybe I just do it in hardware then, firing up the old
Weller. I'd have to buy a bag of varicaps but those are cheap.

Are you trying to sim a VCO? Simulating oscillators is always tedious.

No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.


You could use a diode model, which does include variable capacitance.

https://dl.dropboxusercontent.com/u/53724080/Circuits/Caps/Cap_Sweep.asc

But that's a voltage-controlled voltage source. I'd need a real cap.


Try to get the Skyworks sample kit. It has a lot of varicaps, and many
other cool things.

I'd need the old AM tuning diodes, tons of capacitance. What I need is a
variable range of several hunded pF around a base of 1000pF or slightly
above. Or I have to make Jim's method work but so far no luck. Could
have to do with the durn Windows 7 restrictive file writing "privileges".

If we had all our hardware going I wouldn't need this. It is intended to
give a SW engineer a fake signal in file format that he can plug into
his algorithms so he doesn't have to wait for HW to be done.

I can somehow kludge it with a voltage-variable resistor because in
contrast to capacitors that works in LTSpice. But it won't be pretty.

--
Regards, Joerg

http://www.analogconsultants.com/
 
On Wed, 18 Mar 2015 14:03:07 -0700, Joerg <news@analogconsultants.com>
wrote:

[snip]
No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.


[snip]

I take it you haven't tried my subcircuit?

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
On Wed, 18 Mar 2015 14:13:02 -0700 (PDT), Lasse Langwadt Christensen
<langwadt@fonz.dk> wrote:

[snip]
http://powerelectronics.com/site-files/powerelectronics.com/files/archive/powerelectronics.com/mag/504PET07.pdf

-Lasse

Same way I did my varicap models and Joerg's voltage variable one.
(The varicap model uses a Table to handle the non-linearity of a
varicap.)

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
On 2015-03-18 2:15 PM, Jim Thompson wrote:
On Wed, 18 Mar 2015 14:03:07 -0700, Joerg <news@analogconsultants.com
wrote:

[snip]


No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.


[snip]

I take it you haven't tried my subcircuit?

I have not given up yet but so far I got all kinds of error messages.
The next step would be to try it on an XP machine where I'd have to get
LTSpice going again. XP was IMHO the last known good OS and I've had
error message in other software caused by Windows 7 (meaning they didn't
happen on an XP machine).

--
Regards, Joerg

http://www.analogconsultants.com/
 
On Wed, 18 Mar 2015 14:44:39 -0700, Joerg <news@analogconsultants.com>
wrote:

On 2015-03-18 2:15 PM, Jim Thompson wrote:
On Wed, 18 Mar 2015 14:03:07 -0700, Joerg <news@analogconsultants.com
wrote:

[snip]


No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.


[snip]

I take it you haven't tried my subcircuit?


I have not given up yet but so far I got all kinds of error messages.
The next step would be to try it on an XP machine where I'd have to get
LTSpice going again. XP was IMHO the last known good OS and I've had
error message in other software caused by Windows 7 (meaning they didn't
happen on an XP machine).

What kind of error messages?

If you use the LTspice _symbol_ I made, you need to open the .ASY file
with a text editor and change the path to wherever you've located the
subcircuit definition library.

The latest version, on the website, shows how more clearly.

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
On Wed, 18 Mar 2015 14:03:07 -0700, Joerg <news@analogconsultants.com>
wrote:

On 2015-03-18 1:46 PM, John Larkin wrote:
On Wed, 18 Mar 2015 13:36:27 -0700, Joerg <news@analogconsultants.com
wrote:

On 2015-03-18 11:54 AM, Syd Rumpo wrote:
On 17/03/2015 00:26, Joerg wrote:
Gentlemen,

Setting up voltage-controlled resistors is easy: R=(V(X)+0.01) or
whatever. Works, always did. Doing the same with a capacitor fails with
this error message:

Error on line 6 : c1 n002 0 c=(v(x)+0.01)
Unable to find definition of model "c"

* Unknown parameter "x"
WARNING: Less than two connections to node X. This node is used by V4.
Fatal Error: Missing capacitance value for "C1"

Both sims attached. What gives? Ideas how to make it work? Disregard the
values that wouldn't make sense for the cap here, this is just to find
the principal reason why the control method doesn't work with capacitors.

snip

This is what I did for a time-varying capacitance. In the component
'Value' field, I put Q=(4p/(0.25 +(time*5)))*x which swept the
capacitance from 16pF downwards controlled by the internal variable 'time'.

I can't remember why you need the Q and the x, but you do, and it took a
good while to find out - it seems you can't just vary the capacitance
directly. Replace time with a voltage and the appropriate scaling and
you should be good to go.


Tried it and that completely bungled the linearity when the cap is
inside a resonant circuit. At least no more error messages which is
good. Well, maybe I just do it in hardware then, firing up the old
Weller. I'd have to buy a bag of varicaps but those are cheap.

Are you trying to sim a VCO? Simulating oscillators is always tedious.


No, it's a circuit where a capacitive sensor is employed and I want to
mimic the sensor output. The capacitor itself will be inside a somewhat
resonant circuit so it has to behave like a real and clean capacitor.

Would something like this work?

https://dl.dropboxusercontent.com/u/53724080/Circuits/Caps/Modulated_Cap_1.asc

The cap is modulated by voltage ZZ, which in this case makes the cap
ramp from 1F to 20F. That in turn sweeps the LC ringing frequency
down.


--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com
 
On Wed, 18 Mar 2015 14:55:54 -0700, John Larkin
<jlarkin@highlandtechnology.com> wrote:

[snip]
Would something like this work?

https://dl.dropboxusercontent.com/u/53724080/Circuits/Caps/Modulated_Cap_1.asc

The cap is modulated by voltage ZZ, which in this case makes the cap
ramp from 1F to 20F. That in turn sweeps the LC ringing frequency
down.

<http://www.analog-innovations.com/TankTest_Greenshot_2015-03-18_16-10-12.jpg>

...Jim Thompson
--
| James E.Thompson | mens |
| Analog Innovations | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| San Tan Valley, AZ 85142 Skype: skypeanalog | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 

Welcome to EDABoard.com

Sponsor

Back
Top