LTSpice (windows) - current labelling
LTspice opamps
LTspice includes a folder with many of LT's opamps listed there. Many of these opamps use a symbol you cannot directly observe or edit. But you can hover over the opamp pins and see a designation shown. For example, if I create a new schematic and place the LT1800 on it, then I can hover over all of the pins to see: Ix(u1:In+), Ix(u1:In-), Ix(u1:V+), Ix(u1:V-), and Ix(u1:OUT).
However, if I perform a .OP run, then I will instead see: Ix(u1:1), Ix(u1:2), Ix(u1:3), Ix(u1:4), and Ix(u1:5).
In general, the internal opamp symbol will number the pins 1 through 5 in the order I mentioned earlier: Pin 1 is In+, Pin 2 is In-, Pin 3 is V+, Pin 4 is V-, and Pin 5 is OUT.
Custom opamps
If you are using your own Spice model for an opamp and using LTspice's opamp2 symbol (found in the opamp folder), then your .SUBCKT model will designate the pin identifications. For example, suppose I &quot;cheated&quot; and wrapped up an LT opamp -- the LT1800 -- into the following .SUBCKT:
.SUBCKT MYOPAMP 5 10 15 20 25
XZ1 5 10 15 20 25 LT1800
.ENDS

Then the pins would now be designated 5, 10, 15, 20, and 25 and the .OP run would specify Ix(u1:5), Ix(u1:10), Ix(u1:15), Ix(u1:20), and Ix(u1:25).
Here's the results for a simple run like that:

Force your own designations
Suppose you wanted to make your own labels. You can do this. Start by writing your own .SUBCKT:
.SUBCKT MYMODELNAME MYPIN1 MYPIN2 MYPIN3 MYPIN4 MYPIN5
.ENDS

Within the SUBCKT above, you'd write the necessary lines to fill it out. LTspice will then use your own designations when reporting .OP results.
As a final example, I modified the above case to show the results here;

So you can rename them any way you want.