Is it possible to generate a voltage source that sweeps linearly over a range of frequencies, i.e.: a linear chirp? I’m trying to simulate the ‘sweep’ signal that some function generators have. see attached image.

Thanks,

-May

290px-Linear-chirp.svg|290x194

I am not aware of a readily available linear sweep generator.

As a first trial you might investigate the FFM voltage source (see chapt. 4.1.5 of the ngspice manual). This will give you a sinusoidal modulation of your frequency. And if you use a controlling signal with a very low frequency and a suitable phase offset, then you might explore the “quasi linear” portion of the controlling sine wave.

Best if you make a circuit comprising of the FFM source (library Simulation_SPICE:VSFFM) and run some transient simulations with varying parameters, to see if this somehow fits your needs.

If it is not sufficient, you may construct a chirp generator by assembling a subcircuit with appropriate ngspice components and attach this to a suitable KiCad symbol. First of all you would need to define some specifications, e.g. start time, stop time, start frequency, and stop frequency. Then we need a VCO, for example the ngspice code model 12.2.20 Controlled Sine Wave Oscillator. And we have to control it by a time based voltage ramp, made for example by a pwl voltage source (chapt. 4.1.4 of the ngspice manual).

Ngspice can work with Gnu Octave

Octave can generate chirps easily.

http://ngspice.sourceforge.net/octavespice.html

and

https://wiki.octave.org/Ocs_package

My littel project of a chirp generator with Eeschema/ngspice:

```
* chirp generator by Holger Vogt
* public domain
* bt start time, et end time of chirp
* bf start frequency, ef end frequency of chirp
* code model 'sine' will not accept control value 0, so 1e-12 is used
* r=0 will lead to repeated chirp pattern, cannot be parameterized, so
* has to be removed if a single shot only is required
* to be called by 'XChirp pp 0 chirp bf=1k ef=10k bt=80m et=120m'
.subckt chirp p m params: bf=200 ef=2k bt=30m et=100m
* Start at t=0 with 1e-12, ramp up to t=et-bt with output et, ramp down
* to 1e-12 after another 5% of ramp up time (to catch output 0 again).
* Delay the whole pattern by bt
vcont cc 0 dc 1e-12 pwl ( 0 1e-12 {et - bt} {et} {(et - bt) * 1.05} 1e-12 td={bt} r=0 )
* amplitude is set by out_low, out_high
asine cc %vd(p m) in_sine
.model in_sine sine(cntl_array = [ 0 {bt} {et} ]
+ freq_array=[ 0 {bf} {ef} ] out_low = -5.0
+ out_high = 5.0)
.ends
```

Symbol was generated by checking out Simulation_SPICE:VSIN and adding to it the subcircuit model found in chirp.lib fromChirp.zip (4.0 KB).

Thanks David. I’m not familiar with Octave.

Thanks a lot Holger. This looks very much like what I need. I’m new to KiCad, and circuit simulation in general. I downloaded the zip file you had attached and added the chirp-test-chache.lib file to the symbols library. The other lib file threw an error. Next, I tried to replicate the schematic, but I don’t have a VSIN-CHIRP component. When I search with ‘chirp’ in the component list, I see the chirp library and the Simulation_SPICE:VSIN component. I selected it and tried to edit its SPICE model, but didn’t know which file to select as model? Should there be a .mod file?

Again, taking my baby steps here

Place Simulation_SPICE:VSIN

Double click to open ‘Symbol Properties’ Window --> Edit Spice Model --> Select File -->chirp.lib–>Type: Subcircuit

In line Model: you now have ‘chirp’. Add 'bf=1k ef=3k bt=30m et=70m ’ to get

chirp bf=1k ef=3k bt=30m et=70m

–> ok

In ‘Symbol Properties’ Window, set line ‘Value’ to ‘VSIN-CHIRP’ --> ok

Thanks a ton Holger! Got it to work

and I guess I can change the amplitude by changing the out_low and out_high paramters inside the chirp.lib file.

Thanks again,

-May

You can parameterize the amplitude in the LIB file too. That way you don’t have to keep changing it.

```
* chirp generator by Holger Vogt
* modified by Ste Kulov, so he might've screwed it up, proceed with caution
* public domain
* bt start time, et end time of chirp
* bf start frequency, ef end frequency of chirp
* amp amplitude of chirp
* code model 'sine' will not accept control value 0, so 1e-12 is used
* r=0 will lead to repeated chirp pattern, cannot be parameterized, so
* has to be removed if a single shot only is required
* to be called by 'XChirp pp 0 chirp bf=1k ef=10k bt=80m et=120m amp=1.0'
.subckt chirp p m params: bf=200 ef=2k bt=30m et=100m amp=5.0
* Start at t=0 with 1e-12, ramp up to t=et-bt with output et, ramp down
* to 1e-12 after another 5% of ramp up time (to catch output 0 again).
* Delay the whole pattern by bt
vcont cc 0 dc 1e-12 pwl ( 0 1e-12 {et - bt} {et} {(et - bt) * 1.05} 1e-12 td={bt} r=0 )
* amplitude is set by out_low, out_high
asine cc %vd(p m) in_sine
.model in_sine sine(cntl_array = [ 0 {bt} {et} ]
+ freq_array=[ 0 {bf} {ef} ] out_low = {-amp}
+ out_high = {amp})
.ends
```

That is way more convenient. Thanks Ste!

Dear Holger

I’m trying to get familiar with this chirp generator. I can’t get it to work. I added the library simulation-spice. and I did what you told about editing spice model. After running simulation i get zero for both current and voltage of resistor.

this is the log I get:

## Circuit: KiCad schematic

Error on line 0 :

a.xv1.asine xv1.cc %vd /out 0 xv1:in_sine

MIF-ERROR - unable to find definition of model xv1:in_sine

Warning: Model issue on line 0 :

.model xv1:in_sine sine(cntl_array=[0 2.99999999999999989e-02 7. …

Unknown model type sine - ignored

Reducing trtol to 1 for xspice ‘A’ devices

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Initial Transient Solution

Node Voltage

xv1.cc 1e-12

/out 0

v.xv1.vcont#branch 0

Reference value : 0.00000e+00

No. of Data Rows : 20014

Thanks very much…

This message is typical for an Eeschema/ngspice installation problem. The code models are missing or are not found.

What are your operating system and your KiCad version?

I’m on Debian Buster and KiCad 5.0.2.

Would you mind to update?

In buster backports you will find KiCad 5.1.9 with ngspice-34.

I will. And I will report whether the problem is solved or not.

Thanks very much.

By updating the ngspice engine, my problem is solved. Thanks, dear Holger.