The parts list is generated from the components in the assembly. Take the same screenshot, but with the assembly navigator open.
Also, check the "assembly levels" of the parts list. This option can be changed to show different levels of the assembly. If the 4 items that show up in the list are themselves sub-assemblies, then the "assembly levels" option is probably not set to what you want.
Another thing to look out for is "drafting components"; these are views added from other part files. They add a special icon to the assembly navigator, but they do not appear in the parts list.
and are you able to explain me how to set the assembly levels in correct way? Because you are right, now in part list the subassemblies only appears that why there is only 4 position in the table. Thanks a lot!
Right click on the parts list and choose "edit levels"; a dialog will open with a few toggle options. Have a look at the help file for what each one does:
and I have the last question in this topic. When I try to create part list in the sheet which is show below some error apear. Do you know maybe how I can solvce it?
It's not an error, but a warning. You're attempting to add multiple parts lists to your drawing file.
By default, UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST is set to a value of 1. This value prevents you from inserting multiple parts lists in a single part file and allows ID symbols (balloons) to synchronize with the item numbers in the parts list.
You can set this variable's value to 0, which allows multiple parts lists to be inserted, however, your balloons will not update with any of the parts lists.
The variable is set in the ugii_env_ug.dat file found here: %UGII_BASE_DIR%\UGII, which is typically here: C:\Program Files\Siemens\NX XX.XX\UGII\
It is advised that changes to the OOTB variables are defined in the accompanying environment file: ugii_env.dat (found in the same location as ugii_env_ug.dat), which makes it easier to monitor which variables have been edited.
"It's not an error, but a warning."
I agree that this is more of a warning situation rather than an error; but to make that clear, Siemens should use the warning icon (exclamation point on yellow background) rather than the big red X, and get rid of the word "error" in the message box title bar.
thanks a lot. I have one more question to this drawing. Are you able to answer me why I can not make autoballon on isometric view and detaile view at the same time?