Inventor version 2015 (2016,...) remembers the view parameters (even across sessions) so when you enable thread features in the part view, all subsequent drawing views will have threads enabled automatically. But the default/initial thread features setting is Off.
If you want to enable thread features also for the initial drawing view, you can preset this parameter through the Registry.
This setting is stored in the branch:
Here you can find three bit-coded keys - for part views (IPT), assembly views (IAM) and presentation views (IPN) - specifically BaseViewDefPart, BaseViewDefAssy and BaseViewDefPres.
Each such 32-bit registry key of the type REG_DWORD consists of four bit-octets (four hexadecial pairs) - these octets are coded this way (bit #1 to bit #8):
- Thread feature (1st rightmost bit)
- Interference edges
- Tangent edges
- Hidden line removed
- (not used, 0)
- (not used, 0)
The first of four octets (bit 1-8, first hexadecimal pair, red on the picture) applies to standard projected views (Front - Current - Ortho), the second octet (bit 9-16, green) applies to Iso views, the third octet is not used and the fourth octet (bit 25-32, blue) applies to flat pattern views (sheetmetal).
So enabling thread features for ortho and other part views can be accomplished by setting (use Regedit) the registry key BaseViewDefPart to the hexadecimal value of 01111501 (binary 00000001 00010001 00010101 00000001 - i.e. the bit #1 is On in each octet).
The next Inventor session will have the default part thread features display set to On. For assemblies, repeat the setting in the key BaseViewDefAssy.
Comment by salariua:
You can also customize your template file to preset the features. Open the template "standard.idw", place a view and change the settings while placing or afterwards. Then delete the view and save the template to make this settings persistent.