We an issue with our VCA820 circuit not matching the results we see in TINA
We implemented an AGC loop based on the circuit shown Fig 83 (page 22) of the VCA820 datasheet with some minor changes differences, we simulated the circuit in TINA, but we are not seeing what we expected on the board.
Included with this post are several captures showing the problem as well as the simulation model.
The input to the circuit is a 2V pk-pk signal, 0 offset (shown on inputsignal.jpg)
The input to the VCA820 is a 200mV pk-pk signal, o offset (shown on vca820pin.jpg)
Output of VCA820
The output of the circuit is a 3V pk-pk signal with some offset (shown on opa695pin6.jpg)
The expected output was a 5V pk-pk signal with little to no offset.
Test have been run with multiple boards.
All component values have been verified.
Any input TI could provide would be greatly appreciated.
e2e would not let me attach the TINA file, please contact me if you need it.
Here is the TINA file, zipped
Download the VCA820 TINA-TI Reference Circuit and verify that it is working correctly. Then modify the circuit to your schematic and see if it gives you a correct answer.
I haven't tried this so I can't guarantee that it will work but I think this is your best bet.
Regards, Neil P. Albaugh ex-Burr-Brown
I don't understand your advice, I already have a TINA simulation file for my VCA820 circuit (see previous post), am I missing something? Is it just to verify the VCA820 SPICE model is correct?
That's the idea.
We got the SPICE model from the VCA820 product page, why would it be different (or incorrect) from the one in the reference design?
I have no idea.
We are just trying to find out where the problem is. If the VCA820 model works in the TINA-TI reference circuit but the SPICE model is not working in the circuit that you drew in another circuit simulation software product, it will help identify where your problem lies.
Thank you for your help but I am still confused. We are not using another circuit simulation tool, we've only used TINA-TI. The circuit (based on the datasheet application circuit) was drawn and simulated in TINA-TI (using the TI VCA820 model). The circuit was then implemented on the board, the issue is that what we are seeing in the lab does not match what we see in TINA-TI.
I provided a zipped file with OUR TINA-TI VCA820 circuit, we used to implement.
There was a problem in the loop adjusting the gain control voltage of the VCA820. Once this is resolved and the integrator bandiwdth is increased to pass the signal of interest then the circuit is working properly. See attached simulation file.
Let me know if you have any other questions.
The TINA "reference circuits" were originally created to show that the device model actually does work. So if someone has a problem, they can copy a working circuit and then modify it to their configuration. If that circuit does not work then they know that the problem is not with the device model.
Thanks for solving the problem
I have a few follow-on questions
I am not an Analog guy so I appreciate any additional help you can provide us.
The main error in the circuit from the datasheet is that the input bias current of the OPA820 will drive the integrator to the rail, so the circuit will never work as an AGC circuit.
The new circuit I suggested corrects the functionality. Now the VCA820 gain is always reduced from a maximum gain, so once the maximum gain is set in the forward path, the only possible action is to reduce it. This circuit is very quick at reducing the gain as this is set by the integrator circuit. It is possible to slow this down by increasing the feedback capacitor.
I ran a simulation with 3 different cap value and from that it seems that you want a fast intergrator to control the AGC loop. For 100kHz BW integrator (1.6nF cap), you do see some significant glitch when gain adjustement is needed. Those tend to dissapear as the integrator BW is increase to 1MHz (160pF) or 10MHz (16pF). I ran a longer simulation and saw the same behavior as in the shorter one.
Note that the integrator charges a capacitor through a diode. Only when the signal is greater than the reference voltage does the integrator reduces its output voltage. If the voltage at the output of the integrator is lower than the voltage present on the capacitor C1 then C1 will get lower. If it is higher then a slow recharge, set by R1 and R2, will start.
The integrator is fairly fast, but the control voltage controlling the VCA820 is very slow. Modifying C1, R1, R2 and R12 should be enough to control both discharge and recharge of the AGC circuit.
If you have your modulated signal available, you insert it in a piecewise linear source to simulate with the modulation to see how the circuit behaves. If you need help with the simulation, let me know.
May I ask why there was no errata or update issued for the datasheet? We based our design on the published circuit and now we are facing having to redesign the board in order to fix these issues.
Any idea why our initial simulations looked ok on TINA-TI?
Do you think we can do anything (value changes, etc) with our current circuit design that might get it close to working or do we really need to spin the board (manager is not happy so I have to ask :-) )
For the datasheet, despite all efforts, it happens that a circuit does not work properly in datasheets. Once the problem is recognized, we are updating the datasheet.
I recognized the circuit as not working properly due the the control voltage present on the Vg pin. Since it was stuck at ~4V, the simulation was not working properly. Note that the maximum control voltage pin is +2V.
The circuits are not that different and you should be able to adapt your board to evaluate to the operation of the AGC circuit.
However I am afraid that you will have to spin the board to fix it permanently.
To fix the circuit in your board, the integrator is the same, you will have to replace the diode in front with a short.
On the output of the integrator, you can place a diode in series with the 100ohm resistance. You have missing one pad, but it is posible to bridge the two component with solder if they are placed closed to one another.
That leaves only 3 missing components to be added to the board. If space is limited on the board, you can use wirewond resistance to bridge the gap between the power supply and ground and the Vg pin, same for the capacitor. Since it is the slow portion of the circuit, surface mount resistor are not necessary.
I would recommend a redesign of the board once this circuit has been evaluated in circuit. If needed, I can build the circuit using EVMs, verify the board in the lab and have it shipped to your attention.
All content and materials on this site are provided "as is". TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with regard to these materials, including but not limited to all implied warranties and conditions of merchantability, fitness for a particular purpose, title and non-infringement of any third party intellectual property right. TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with respect to these materials. No license, either express or implied, by estoppel or otherwise, is granted by TI. Use of the information on this site may require a license from a third party, or a license from TI.
TI is a global semiconductor design and manufacturing company. Innovate with 100,000+ analog ICs andembedded processors, along with software, tools and the industry’s largest sales/support staff.