Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

problem with a colpitts VCO in ADS

Status
Not open for further replies.
asoom

asoom

Full Member level 1
Joined
Dec 28, 2007
Messages
99
Helped
15
Reputation
30
Reaction score
1
Trophy points
1,298
Location
jordan
Activity points
2,032
hi all,
i am implementing a colpitts VCO using the ADS2006, i tried simulating the schematic with the harmonic balanced simulation but i couldn't get the expected output. instead i got a dc output! i looked in a lot of the harmonic balanced tutorials and guides and i couldn't figure out the problem. am afraid that there's something wrong with the schematic itself (THOUGH I COULDN'T FIND ANY), so i included an attachment of an image of the design file of my schematic, tried to attach the design file itself but it didn't work. if there's anybody that have an idea of 'what is the problem', i will be so thankfull for the help!

thanx alot in advance
 

there is no problem in the schematic.
do you have wrong output frequency or other question?
 

the problem is that Vout (on the inductor) was a dc voltage, and the current in it was a normal sinusoid! what is expected is a frequency modulated version of the sinusoidal signal of the applied source. actually this circuit must work as an FM transmitter around an oscillation frequency of 100MHz, and the antenna would be connected directly to the inductor. so the modulated signal should appear instead of that DC output!
 

Hi

Your "Vout" looks to me to be connected directly to the Vdc=9V.
I can not see you having any sinusoid voltage there other than a DC voltage of 9V.
 

actually there is another sinusoidal source, which is labeled (SRC7) of the type V_1 Tone. this the voltage source that should be changing the frequency of the colpitts oscillator!
 

1) remove this SRC7 now ,
2) u need to add the osc_probe , check it in HB

3) did u check the HB tutorial about oscillators , and make all oscillator simulation options

could u upload ur project , so we can check it

khouly
 

why would i remove the source SRC7? it is the message signal that am going to use to modulate the carrier signal produced by the oscillator! actually the hardware implementation of this schematic will include a mic or so instead of this source, as the purpose from this circuit is to transmit voice to FM radio (FM transmitter).

i tried to use an oscillator probe but there was no difference, i also read the oscillator design guide and HB guide provided by Agilent but found nothing!

here is the design file of the schematic, i think that it is enough.
thanks for all those who replied so far:D
 

hi guys,

can't anybody help me with this problem:cry:
 

Here is a simulation I did on a similar circuit but not with ADS. You might find some info helpful



I attempted to open your project in ADS but it contains no networks or results. Maybe you have not exported the project correctly.
 

    asoom

    asoom

    Points: 2
    Helpful Answer Positive Rating
Here is a simulation of the osc part in ADS to give you some idea. Shows oscillation around 100MHz at about 10mW output. You can see that Vout on the tank goes above 9V as expected by theory.
 

then there isn't any problem with the oscillator part. actually i can't find any problem with the whole circuit! i must obtain the same output as yours but with the frequency varying according to src7 which is my message signal. instead, this is the output that i've obtained.

is there anything wrong with my simulation setup? i tried almost everything and the output didn't change!

the first time, i uploaded the desing file only, you can copy the design file into a new project. anyway here's the project. hope it will work this time. i will be so thankful if you review it.
 

asoom you connect the all capacitor in revers form why ?

you use the transistor but there is no model for it why ?

i am using ADS2004A , why your transistor look different here about collector terminal. ?

Added after 7 minutes:

can you upload the your complete design here.

COMM_prj.rar does not contains anything .

i am interested in this vco so , tell me about your transistor model and gain ?
 

thanx alot, i didn't notice that am connecting then in that way. unfortunately, i fixed them but nothing changed:cry:

now about the transistor, at first i didn't know which one to use. so i referred to tha examples provided by the ADS, and i found that they used this transistor in (learningOsc_prj) where they simulate a vco with HB simulation. so i used the same transistor.

i tried to use the transistor with the model, it gave the same results. by the way am using the ADS2006A.

I uploaded the design file before. you can create a new project and copy the design file into it. i also uploaded the project, am sure that it contains the design in the networks folder.
 

what you upload i simulate it , and what i get , i upload it.

ok , now what is you problem


ok i get , you want the variation in output with respective to the vin ...using HB tool ok..

i try my best to get it .
 

asoom said:
then there isn't any problem with the oscillator part. actually i can't find any problem with the whole circuit! .
Click to expand...

Your values are suspect. 8O

Your tank circuit is a 1uH to resonate with 40pF which will give a very low frequency. This will also give a low Q tank with bad stability and bad phase noise. I assume you need it to transmit somewhere between (88-108MHz) commercial band. At your frequency your C5 may be much too small to provide enough feedback to sustain oscillations. Your emitter degeneration resistor is way too big (100k)?? It would be better to couple the baseband via a capacitor between your first transistor o/p and osc i/p

Added after 3 hours 27 minutes:

Here is the modulated spectrum showing frequency deviation below & above the carrier. Notice that it is very non linear and there are AM and FM components generated in this simple base modulated circuit. You must use envelope simulation to get to this result.
 

why do you think that the frequency will be very low? actually in colpitts oscillators two capacitors are used and they are treated in series, which means that the tank circuit will include the 1uh to resonate with the equivalent of 40pf and 2.7 pf. this will give a resonant frequency of 100MHz which is within the required band.

this circuit was implemented by hardware components and it worked successfully. i wish i could know what is the problem with the software simulation of it. am i using wrong values for the LC tank? or is there something wrong with my simulation setup? something in the connections? what is the problem?!

i tried your LC tank values, also nothing changed. did you try the HB simulation with the schematic you uploaded? if yes, did you get the expected output?
 

All my results are from the circuits I posted.

Go and make sure about your formulas. F= 1/(2Π√LC) ≈ 25MHz

The circuit you show will try and oscillate around 25MHz. The 2.7pF capacitor has little effect on the final frequency and its main function is to provide feedback. At 25MHz this value is way too small in any case. The hardware you tested will have harmonics. So you probably picked up the fourth harmonic of your oscillator on a receiver. The reason it may have oscillated at all is because of stray capacitances introduced in construction.

With your tank values and (4.7pF feedback cap + 220 Ohm emitter resistor), this is what a simulation of your output looks like below. It fails to start oscillating with a 2.7pF ideal component value.

If you look at a open loop linear simulation of your circuit you will see that the area where you have any gain for oscillation to start is around 24MHz. This is also the resonant frequency of your tank values as the rapid phase shift at this point proves.
 

thanx alot, it seems that i misunderstood the idea. i thought that the 2.7pf capacitor is included within the resonant circuit and i used (c8*c5)/(c8+c5) in calculating the value of L required to obtain a 100MHz resonant frequency. i did that because colpitts oscillators should use two capacitors so i thought it's included.

i changed the value of L to 63.325 nH. and tried the HB again but still didn't get the output. would you plz try the HB simulation on my circuit with the new value of L.

thanx alot
 

If you set your HB controller like mine there is no reason you should not get the same results.

Did you fix up the 100k resistor on the emitter?
 

yes i fixed it to 220 ohm. can u tell me your HB controller's main settings.

Added after 2 minutes:

yes i fixed it to 220 ohm. can u tell me your HB controller's main settings.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top