# LTspice Frequency Response Analyzer (FRA)

This post is a continuation of this question.

LTspice recently introduced a new feature called frequency response analyzer, see the image below.

The green box shows the symbol for FRA. If you click on the FRA the second image pops up for configuring the FRA. Then if you click on 'Help me to configure this for a switching regulator', the third window comes.

I have some questions regarding the third window.

1. How do I get Approximate Closed-Loop Bandwidth of a switching regulator? Is this information available in the datasheet?

2. From where I will get Approximate common mode voltage at FRA device?

As per Lars' answer, the part circled in yellow is the rise time. Please correct me if I am wrong.

This is the example AD circuit for the frequency response analyzer (FRA):

The FRA symbol is placed into the feedback path. The common-mode voltage at that point is the output voltage of the switching regulator, 5 V in this example.

For the closed loop bandwidth you could look into the datasheet for a typical transient response graph. This is from the LT8618 datasheet for example:

From the 10% to 90% rise time after the load step you can calculate the bandwidth: $$BW = \frac{0.35}{t_{rise}}$$

My approximate reading from the graph is a rise time of 100 microseconds. This results in a bandwidth of 3.5 kHz which is relatively close to the data in the example:

• Where does the value 0.35 come from ? Apr 8 at 19:19
• As far as I'm concerned it is an emperical estimation. You can find it in many books and websites. Apr 8 at 19:34
• @LarsHankeln,I updated the question.Could you please confirm my understanding is correct or not
– Hari
Apr 9 at 5:11
• @Hari Yes, that is correct. Apr 9 at 5:27
• @Hari I updated the graph in my answer to clarify. To be precise, you would try to measure the 10% to 90% rise time to calculate bandwidth with the formula. But approximations should be fine for the FRA anyway. Apr 9 at 5:50