I interpret roboya’s post as that he has made a 3D shape and knows how to work with it, but his problem is that he has to add the 3D settings to each of his 16 opamps separately.
In Eeschema there is:
Eeschema / Tools / Edit Symbol Fields
spreadsheet to easily copy attributes from one object to the other, and there is no equivalent for this in Pcbnew. (Hopefully it will come someday…)
At the moment the best workflow for this is to put the 3D setting for your component into the library of that object, and then:
Pcbnew / Tools / Update Footprins from Library.
It is important to realise that each component in Pcbnew is COPIED from some library into the PCB file, and from thereon it is a separate entity.
If your board has 100 resistors, and you move the silkscreen text of a resistor, it changes only for that resistor.
If you move or modify a pad on one of the resistors, only that resistor is effected.
This makes it pretty easy to make small modifications to Footprints, without having to bother with library management. Those small changes are often very specific for a project and not usefull to put in a library.
Another way to change the 3D settings of all your opamps is to simply edit the project.kicad_pcb file with a text editor, and copy the settings from one opamp to all the others. All KiCads files are text based and weird hacks can often be done relatively simply in a text editor. In a text editor, the complete definition of a (THT) resistor looks like:
(module Resistor_THT:R_Axial_DIN0204_L3.6mm_D1.6mm_P2.54mm_Vertical (layer F.Cu) (tedit 5AE5139B) (tstamp 5C9BC78F)
(at 180.078494 101.341256 180)
(descr "Resistor, Axial_DIN0204 series, Axial, Vertical, pin pitch=2.54mm, 0.167W, length*diameter=3.6*1.6mm^2, http://cdn-reichelt.de/documents/datenblatt/B400/1_4W%23YAG.pdf")
(tags "Resistor Axial_DIN0204 series Axial Vertical pin pitch 2.54mm 0.167W length 3.6mm diameter 1.6mm")
(path /5C69C2AF)
(fp_text reference R9 (at 1.27 -1.528744 180) (layer F.SilkS)
(effects (font (size 1 1) (thickness 0.15)))
)
(fp_text value 4.7k (at 1.27 1.92 180) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
)
(fp_text user %R (at 1.27 -1.92 180) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
)
(fp_line (start 3.49 -1.05) (end -1.05 -1.05) (layer F.CrtYd) (width 0.05))
(fp_line (start 3.49 1.05) (end 3.49 -1.05) (layer F.CrtYd) (width 0.05))
(fp_line (start -1.05 1.05) (end 3.49 1.05) (layer F.CrtYd) (width 0.05))
(fp_line (start -1.05 -1.05) (end -1.05 1.05) (layer F.CrtYd) (width 0.05))
(fp_line (start 0.92 0) (end 1.54 0) (layer F.SilkS) (width 0.12))
(fp_line (start 0 0) (end 2.54 0) (layer F.Fab) (width 0.1))
(fp_circle (center 0 0) (end 0.92 0) (layer F.SilkS) (width 0.12))
(fp_circle (center 0 0) (end 0.8 0) (layer F.Fab) (width 0.1))
(pad 2 thru_hole oval (at 2.54 0 180) (size 1.4 1.4) (drill 0.7) (layers *.Cu *.Mask)
(net 30 SCL))
(pad 1 thru_hole circle (at 0 0 180) (size 1.4 1.4) (drill 0.7) (layers *.Cu *.Mask)
(net 8 VCC1))
(model ${KISYS3DMOD}/Resistor_THT.3dshapes/R_Axial_DIN0204_L3.6mm_D1.6mm_P2.54mm_Vertical.wrl
(at (xyz 0 0 0))
(scale (xyz 1 1 1))
(rotate (xyz 0 0 0))
)
)
Even without looking at the documentation of the file format
https://kicad.org/help/file-formats/ it’s pretty trivial to identify most things. The 3D settings are on the bottom, with a filename, and settings for offset, scale and rotation.