how to resolve PSPICE error

[f.nasr]

I would like to run an AC sweep for a very simple circuit (Please see the attached file). Unfortunately the following errors occurred:

L_L2 N04540 0 .10976mH

R_R3 N04968 N02907 10.7849 TC=0,0

C_C6 N04540 N04968 7.6091u TC=0,0

C_C5 0 N02907 .64335u TC=0,0

I_I1 N04863 0 DC 0Adc AC 1Aac

L_L3 N04858 N02907 1.989m

L_L4 N04863 N04858 3.933m

C_C7 0 N04858 1.099u TC=0,0

**** RESUMING test.cir ****
.END

ERROR(ORPSIM-15142): Node N04968 is floating

ERROR(ORPSIM-15142): Node N02907 is floating

ERROR(ORPSIM-15142): Node N04863 is floating

ERROR(ORPSIM-15142): Node N04858 is floating

Although I have checked the circuit several times in order to resolve the problem, I have not succeeded. Does anyone know how to solve it?

 

[FvM]

SPICE performs a DC operation point analysis previous to AC analysis. The said nodes have no DC path to ground and thus cause an error in DC analysis.

Solution: Add a high resistance (e.g. 1G, can be even more) from one of the floating nodes to ground.

 

[mvaseem]

All the nodes to going to ground have capacitor in path, leaving no path for DC current to ground.
As FvM said, you need to add high resistance like {1/GMIN} which equals 1000 Gohm, from one of the nodes to ground, for successful operating point calculation.