there is a pivot/hole component positioning command

[Giancesa]

I don't know if sw has a positioning command touching two turns, one of a screw, one of the hole, automatically positioning the screw to its hole. for this now I do so: first I give concentricity and then I support the underhead of the screw on the plane of the piece. I wonder why inventor had it and it was convenient. Thank you.

 

[MassiVonWeizen]

select the two edges and have the coincidence and concentricity

 

[SperX]

I think you have to set the screw with the automatic mathematician.

 

[Giancesa]

I tried by clicking the two edges, but you also need to click "center profile". the thing speeds up by clicking directly "centre profile" when opening the quick menu

 

[Atreiou]

If you select the two edges and give only the coincidence in basic materials?

cmq after years of assembly of this type (piping) in the end I decided that it is better to give the classic 3 couplings, concentric, with accident, and parallel to avoid rotation (or to the maximum block rotation, that in 2020 is comfortable and appears just after giving concentricity)

 

[MassiVonWeizen]

If you select the two edges and give only the coincidence in basic materials?

only works if the two diameters are equal

 

[MauroM]

I don't know if sw has a positioning command touching two turns, one of a screw, one of the hole, automatically positioning the screw to its hole. for this now I do so: first I give concentricity and then I support the underhead of the screw on the plane of the piece. I wonder why inventor had it and it was convenient. Thank you.

Unfortunately the same command is not there, but you can do this:
- hold the alt key
- click left and hold the underhead edge of the screw
- drag the screw and approach the edge of the hole, at this point should "capture you" the point
- release everything and create the two constraints

Mature

 

[re_solidworks]

I don't know if sw has a positioning command touching two turns, one of a screw, one of the hole, automatically positioning the screw to its hole. for this now I do so: first I give concentricity and then I support the underhead of the screw on the plane of the piece. I wonder why inventor had it and it was convenient. Thank you.

you must define mating rules in the screw (or pin). open the screw, select the circular edge lying on the plane that must go into contact (subhead) and then go on "put->geometria reference->regole coupling. confirm and save the component. Now when you insert it, just touch a circular edge, it is concentric and coincident position. If it is oriented to the reverse, you can turn it with the tab button during positioning.
Let me know if the result is what you meant.