NX Create a hole pattern to autofill an irregular shape surface

Does NX have an Autofill option for creating pattern like SolidEdge? 

Supposing you have an irregular shape part like this:

And you want to create a pattern of the hole to autofill the surface of the part without specifying how many copys of the hole. Can it be accomplished in NX?

Solution

Yes you can certainly do this from using Pattern Face command:

Insert --> Associative Copy --> Pattern Face ->Set Dialog Options (upper left corner)  to Pattern Face (More)
--> select the hole face --> accept the center point of the hole as Reference Point --> set your Pattern Definition Layout --> under Boundary Definition, set Boundary to Face --> toggle on Simplified Boundary Fill  --> set Margin Distance (from the edge of your part to the hole) -->  select Curve --> select the face of the part.

Simplified Layout --> Set the Layout (Default to Square) --> Set the Pitch distance ( distance between the holes) --> Apply

Note: You might get this alert:

If your Pitch Distance defaults to 1, you might need to change it appropriately.  In this case, the hole is 1 inch in diameter, so after changing the pitch distance to 1.5, you will no longer get this alert.

The Preview:

--> Apply

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: windows
OS Version: 1064
Product: NX
Application: DESIGN
Version: V1911
Function: FEATURE_MODEL

Ref: 001-9764904