if i have one main assembly .prt and in that perticular folder i have many child members .now i want to show only single part file in which customer can see complete assembly.
You can do what you describe.
Here is an assembly of a Toggle clamp.
In the 'Assemblies' toolbar click on 'Wave Geometry Linker' this tool copies assembly parts into the work part.
When the dialogue opens select Type 'Body'
Select all parts of the assembly you want to copy to the work part and make sure you have 'Hide Original' checked.
You now have a copy of the parts in the work part.
Go to, File > Export > Part
Once the Export Part dialogue opens.
1. Specify the new part name
2. Select all the parts of the assembly you want to Export.
Check 'Remove Parameters'
Check 'Copy if Referenced'
You now have a single .prt file of your assembly, the parts in this file will not have any parameters and will not be associated with any other part.
I don't think so though...but u could try another way!
Try to EXPORT your assembly file into IGES/STEP (can be done in NX itself), which will come out as a single file. Then your customer could use IMPORT (also in NX itself) IGES/STEP and all the file will convert back to NX assembly + part file. It will not take that long and not really a hassle.
If you are worried that the customer will not know how to IMPORT the file, then just Winzip/Winrar them.....
Under my account, I got a file for Rigid Clamp, which I did in NX. I export and upload an IGES format too. You could try with that to see whether u prefer using that method.
Its called "create assembly" but all 'parts' must be in the appropriate 'directory'
You could also just export a parasolid.
export parasolid and save to other name