10 MHz Voltage to frequency converter required !!!

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
Dear Respected all,

Hope you all are fine and enjoying your life. Here i am interested to ask for one favor on urgent basis. I am trying to design 10 MHz V2F converter, but failed to get good results after simulation, for designing and simulation purpose LTspice used, i am beginner for this area but i need. if any one can provide me right circuit then i shall be highly grateful to him/her for this act of kindness.. i had also found some circuits from internet, because of lack of information couldn't successful ....

A prompt reply will be highly appreciated !!!


With Humble Regards
 

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
What range of frequency will be input to this converter? Or: what is the maximum and minimum frequency?
Dear Marley,

Thanks you very much for your kind reply, actually i have found one circuit from ;
https://www.analog.com/media/en/technical-documentation/application-notes/an72f.pdf

At page no. 25, one circuit related to voltage-to-frequency converter. A 0V to 2.5V input produces a 0Hz to 10MHz output with 40dB of dynamic range, but i am unable to find the desired frequency at the out put. I shall be highly grateful to you for this act of kindness if you can some help for me ...

Regards
 

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
hi,
Please post your LTSpice asc file, so that we can check the circuit.
E

Dear ericgibbs,

Thanks you very much for your kind reply, actually i have found one circuit from ;
https://www.analog.com/media/en/technical-documentation/application-notes/an72f.pdf

At page no. 25, one circuit related to voltage-to-frequency converter. A 0V to 2.5V input produces a 0Hz to 10MHz output with 40dB of dynamic range, but i am unable to find the desired frequency at the out put. for this purpose i am forwarding you my schematic design, but remember i am confused about frequency and type of input signal and and the connection of pins 4 & 5. I shall be highly grateful to you for this act of kindness if you can some help for me ...

Regards
 

Attachments

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
Dear jpanhalt,

Thank you very much for your kind reply. These ICs also reasonable , but i am worried about there no spice model available in LTspice for simulation ... what can i do in this situation ?? Please suggest ...

Regards
 

jpanhalt

Joined Jan 18, 2008
8,717
I haven't checked specifically, but there are LTSpice groups with archives of various chips. I don't participate in them. When I need something that is not in the LTSpice library, I just search to see whether someone has developed a model.
 

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
Hi 1114,
What is the purpose of Q4 and Q5 transistors in the simulation circuit.?
E
Dear ericgibbs,

I think use for current control, but frankly speaking i am also not sure, but one important thing i wanna tell you that at output i need frequency of 10 MHz (max) , if you think some change is needed.. you can suggest me ... also tell me the input signal's frequency and type ...

Thanks
 

eetech00

Joined Jun 8, 2013
1,835
Hello

See simulation below for following comments:

1. There were a few wiring errors.
2. I used the 74HCT library for the logic inverters...74HCT04. This is downloadable from the LTspice group library.
3. I used a 1N5711 as a substitute for the 1N5712. (Couldn't find a model).
4.This is a voltage to frequency converter. So the input can be a steady DC voltage that will be converted to a frequency.
Your simulation used a pulsed DC input source to speed up the simulation. I used a steady DC source.
5. I used .meas commands to measure the output frequency instead of using the graph. This make it easy and uses LTspice to do the measurement work. :)6. LTspice performed multiple sims while stepping the R2 value from 2k to 10k in 2k steps. From this I determined in order to tune the circuit to 10 Mhz FS, I needed to reduce R1 to 5k. The measurement results are shown in the Error log file.

I didn't spend a lot of time analyzing the circuit so you'll have to work out the details...
:cool:

eT

1578680122381.png
 

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
Hello

See simulation below for following comments:

1. There were a few wiring errors.
2. I used the 74HCT library for the logic inverters...74HCT04. This is downloadable from the LTspice group library.
3. I used a 1N5711 as a substitute for the 1N5712. (Couldn't find a model).
4.This is a voltage to frequency converter. So the input can be a steady DC voltage that will be converted to a frequency.
Your simulation used a pulsed DC input source to speed up the simulation. I used a steady DC source.
5. I used .meas commands to measure the output frequency instead of using the graph. This make it easy and uses LTspice to do the measurement work. :)6. LTspice performed multiple sims while stepping the R2 value from 2k to 10k in 2k steps. From this I determined in order to tune the circuit to 10 Mhz FS, I needed to reduce R1 to 5k. The measurement results are shown in the Error log file.

I didn't spend a lot of time analyzing the circuit so you'll have to work out the details...
:cool:

eT

View attachment 196612
Dear eetech00,

Thank you very much much for your kind help. here i would like to ask for one more favor, please send me the lib file of 74 hc coz in fact my file is not very good ... and also the schematic of cct which one you designed by your self ... I shall be highly grateful to you for this act of kindness..
 

Bordodynov

Joined May 20, 2015
2,495
Hello eetech00.
.MODEL 1N5711 D (IS=19.7n N=1.51 BV=93.3 IBV=50n RS=6.27 CJO=1.8p VJ=.75 M=.333 XTI=2 EG=.69 TT=10.8p Iave=50mA Vpk=70 type=Schottky)
.MODEL 1N5712 D (IS=7.02E-09 N=1.25 BV=2.66E+01 IBV=5.00E-08 RS=8.77E+00 CJO=1.20E-12 VJ=.75 M=.333 XTI=2 EG=.69 TT=2.52E-11 Iave=50mA Vpk=20 type=Schottky)
 

eetech00

Joined Jun 8, 2013
1,835
Hello eetech00.
.MODEL 1N5711 D (IS=19.7n N=1.51 BV=93.3 IBV=50n RS=6.27 CJO=1.8p VJ=.75 M=.333 XTI=2 EG=.69 TT=10.8p Iave=50mA Vpk=70 type=Schottky)
.MODEL 1N5712 D (IS=7.02E-09 N=1.25 BV=2.66E+01 IBV=5.00E-08 RS=8.77E+00 CJO=1.20E-12 VJ=.75 M=.333 XTI=2 EG=.69 TT=2.52E-11 Iave=50mA Vpk=20 type=Schottky)

Thanks Bordodynov!

eT
 

eetech00

Joined Jun 8, 2013
1,835
Dear eetech00,

Thank you very much much for your kind help. here i would like to ask for one more favor, please send me the lib file of 74 hc coz in fact my file is not very good ... and also the schematic of cct which one you designed by your self ... I shall be highly grateful to you for this act of kindness..
HI

I'm attaching the schematic and have replaced the 74HCT04 with the native LTspice inverters. I've defined some parameters on the schematic that I've used in the inverters. I've also used the diode model provided by Bordodynov.

You will find that the frequency has changed using the 5K resistor. That is because the behavior of the native inverter is not as good as the 74HCT04 modeled in the 74HCT library. The 74HCT library can be downloaded from the LTspice group at groups.io.

eT
 

Attachments

Thread Starter

Nomi 1114

Joined Dec 4, 2017
86
HI

I'm attaching the schematic and have replaced the 74HCT04 with the native LTspice inverters. I've defined some parameters on the schematic that I've used in the inverters. I've also used the diode model provided by Bordodynov.

You will find that the frequency has changed using the 5K resistor. That is because the behavior of the native inverter is not as good as the 74HCT04 modeled in the 74HCT library. The 74HCT library can be downloaded from the LTspice group at groups.io.

eT

Dear eetech00,

Thank you very much for your kind cooperation ... you helped me a lot.. i don't have appropriate words to say thanks but i am really grateful to you ...
 
Top