SIM900 Footprints do not match in Eagle
The Eagle part you are using is badly designed. The pins are too wide and not centered correctly, and it doesn't have the required routing keep out areas.

For the correct dimensions, refer to the SIM900 Hardware Design datasheet figure 38: "recommended PCB decal". The pads should be 1.6mm long and 0.6mm wide, placed 12mm from the center of the part. Rectangles should be placed in in the tRestrict layer from (-7.3, -2.8) to (-1.7, 2.8) and (-1.5, 7.0) to (0.5, 9.0), to keep these areas clear.  

To edit the footprint you must open the sim900 library and edit the package. Group select each row of pins and move them 12mm from center. Use the 'Change' command to make the pads 1.6 x 0.6mm and 100% round. View pad properties to make sure the dimensions and positions are correct.    

The corrected package should look like this:-