I have multiple issues with LTspice. Take this trivial example:
XU1 N002 N001 vcc 0 N001 N003 ADA4807
V1 vcc 0 5
V2 N002 0 PULSE(0 1 0 0 0 0.5m 1m) AC 1
R1 N003 vcc 1k
C1 out 0 1p
R2 out N001 1
;tran 2m
.ac dec 1 100 1000Meg
.lib ADI.lib
.backanno
.end
tran works fine:
But ac gives me bogus results - like -47 dB "gain":
As mentioned by just about everyone in the comments, your op amp doesn't work because your DC bias point is 0V and the op amp will only work for inputs between its rails (0V and 5V).
Your options are either: 1) Use positive and negative op amp rails, or 2) Bias the input AC voltage to between the two rails, e.g. 2.5VDC.
As seen below, with the DC bias point set at 0, I get similar broken behavior (although its a bit different since I used a different op amp)
If I add a 2.5V DC offset to the AC input, I get the expected behavior:
EDIT: See also The Photon's answer describing why the minimum output voltage limits you in this case.
The ADA4807 input range includes the negative and positive rails. In fact it allows input 0.2 V beyond either rail.
Further, in the Theory of Operation section the datasheet says,
Specifications like input bias current, offset voltage, etc., might not be maintained with the input biased at the negative rail, but in general this op-amp should still act like an op-amp in that condition.
However, the minimum output voltage is 0.1 V above the negative rail. You'll also notice that the minimum output voltage in your transient simulation was about +0.1 V.
Therefore a follower configuration cannot maintain negative feedback when the input is at or below the rail, and the op-amp will be saturated at this bias point.
In saturation, very low AC gain is expected, and this is reflected in your AC simulation result.
If you arrange to have a negative supply available, or bias the input at least 0.1 V above the negative rail, you should see a gain of 1 for this circuit.
For AC analysis, LTSpice constructs a linear (small signal) model of your circuit considering the DC operating point [*]. Datasheet of the device ADA4807 says that this is a rail to rail input/output opamp, though the LTSpice model doesn't seem to agree with it. Especially the ground rail, transient output could not go below about 0.07V however it reaches 1V perfectly. Based on this, for the opamp model that cannot amplify at ground DC level, the AC simulation seems fine (i.e. in accordance with the transient output).
To resolve, you may add a DC bias to your AC signal source via its DC voltage property (should be at the upper right corner of the properties window of signal source V2).
A better and widely useful way of supplying such biasing conditions is as follows: You may AC couple your input signal via a large (1GF) capacitor, and provide your DC bias (like Vcc/2) via a large (1GH) inductor, as shown in the below figure:
simulate this circuit – Schematic created using CircuitLab
[*] LTSpice uses DC operating point analysis to obtain those DC voltages at all nodes. In your circuit, AC analysis sees 0V-DC at the + input of the opamp since no other DC bias is applied, which supposedly prevents amplification.
