Hi Abbas,
I'm convinced you don't go the logic way when copying a package from one library to another.
If your PC doesn't write windows will come up with a severe error message like "disk full", "can't read from FAT" or similar messages.
You can't copy one library to another. Moreover you must copy and paste parts (components) from one to another.
Please follow these steps and I expect a success report only.
Open the library I posted and get the "package". Check if all necessary layers are active, 'pads' (layer17), 'tPlace' (layer21) and if necessary for SMT components also 'top' (layer1).
Group the entire package including the texts >NAME and >VALUE. Use the scissors symbol for "CUT" and hit the green traffic light next to the STOP symbol. When the green light extinguishes the package has been stored to the paste buffer.
Close that library and open the one you want to copy the package to. Select 'package' --> 'new' and type in the name "SOT23-6".
Next look for the brush symbol with a bit of yellow paint. Hit that and throw the package out of the paste buffer onto the screen. (with the XY-position centered on the package or a reference pad)
Hit save and you're finished. Opening the library again the package name should be contained in the list.
However the package is a lone package, not assigned to any 'device'.
Click 'symbol' and create a symbol of the IC you want to put into the SOT23-6 package. Do that the normal (personally preferred) way numbering the pads and writing the pin name into the box. Click 'visible' and activate 'pads'. If you do that before placing any pin on screen the pin displayed shouldn't have any fancy name attached to it like 'P$2'. See the screenshots for details.
Finish and save the symbol you've just created.
Next create a device, which must contain of a symbol and a package.
Click device --> new and type in the device's name, e.g. 'ABBAS-01'
Next 'ADD' the symbol you already have made and assign the appropriate package.
The device is now almost finished. However Eagle has no faint idea of how to assign pins to pad numbers. So next you must 'connect' pins and pads.
The example shown carrying the pin name /MCLR has to be assigned pad number1. You won't have to check the data sheet again if you use the method I described when creating the symbol. Just connect the same numbers like G$1 -> to pad 1 (G$1 is the pin name which Eagle assigns automatically if you don't explicitely give a pin name)
When pin and pad assignment is finished save your work with a new component ready to use in the schematic and board editor.
Regards
Boncuk