THS3491: Driving capacitive load simulation problem

Hello Shel,

Could you share your schematic or simulation file?  I know that capacitive loading can cause stability issues rather easily; you may want to review the THS3491 datasheet and examine recommended values and loading conditions.  

I can take a look at your circuit and examine potential solutions once I have more information.

This prior thread also addresses capacitive loading: https://e2e.ti.com/support/amplifiers-group/amplifiers/f/amplifiers-forum/792461/ths3491-about-the-output-capacitance-and-stability

Best,

Alec

I reviewed the data sheet and related posts. Here's my schematic:

I used large valued resistors and a large series resistor to try to tame the simulation but it's still there. It's looking to me like this may be a model issue. I'm not using Tina, I'm using regular Spice. Even a 10pF cap is problematic. If I remove the cap entirely the circuit works as expected. I've never actually seen a good simulation with capacitive loading in the entries even though the issue has come up.

Thanks,

Shel

Working on this further, I was able to get rid of the oscillation by simulation the power supplies with output impedances under 1 milli-ohm. Even 5 milli-ohms showed oscillations on the output. 1 milli-ohm seems excessively low. I hope the real parts aren't this sensitive?

Shel 

Hi Shel,

keep in mind that a 10pF cap presents an impedance of 18Ohm at 900MHz, and a 100pF capacitance of only 1.8Ohm. So, you will short circuit the output of THS3491 when connecting such a cap from the output of THS3491 to signal ground. Also, the Spice models are intended to be used in standard applications. Short circuiting the output is no standard application 

Kai

Thanks Kai. The data sheet shows driving a 1 uF cap with a 1 ohm series resistor. I was driving 10 pF with a 10 ohm series resistor. The amp is supposed to handle that easily.

Hi Shel,

I can confirm instability with non-zero supply voltage impedances in TINA-TI too.

Can you tell more about your application? What is your input signal? Why do you want to add a capacitive load of 100pF?

Kai

Thanks, Kai, I appreciate your confirming that. I'm driving an RF FET with a modulated 80 MHz square wave. At these frequencies, the FET presents a capacitive load. The circuit simulation seems to work as long as I maintain the very low source impedance for the power supplies.

Hi Shel,

I would would say that the instability seen in the simulation of transient analysis with non-zero supply voltage impedances seems to be a model issue. Whatever circuit I simulate, with or without capacitive load, whenever I increase the supply voltage impedance(s) from zero on, the simulation stops working properly. Only when I add an ideal decoupling capacitance directly at the supply voltage pins of THS3491 the simulation works properly again.

I would say that your circuit is still stable:

Increasing the isolation resistor R1 will enhance the stability:

shel_ths3491.TSC

Kai