Altium Designer 3d modeingl frustrating question .

Altium Designer 3d modeingl frustrating questions .

Hi to group

I have some questions that confuse me in AD14 . Is the best way to use Altium with a database linked to sch,pcb,pcb3d libs or an integrated library containing everything ?.I have experimented with database and find it very comfortable . I haven't managed to view any 3d model though altough my links are correct .Does altium 14 support legacy 3dpcblib?. Can someone describe 3d models in a separate 3dlib ?. How can we add multiple step models in one footprint and select during schematic placement which one to use ?. Is this possible ?.

You should only have one 3D model per footprint, otherwise you are going to make life complicated.

You can have multiple footprints per schematic symbol though. And when you place the symbol into the schematic, you can open the symbol properties and choose which footprint to use. For instance, our 0402 parts contain both a standard IPC footprint, and a high density version with minimal silkscreen and decreased pad size; default set to the IPC version. After I place the part in the schematic, I can open the symbol properties and select the appropriate footprint from the model list at the bottom.

In your case, if you wanted the same footprint, but different 3D models, you could create two copies of the footprint and place one version of the step model on the first footprint, and the second version of the step model on the other. Then just add both footprints to the desired symbol in your library and choose the appropraite footprint when the symbol is placed.

In regards to the libraries, independent discrete libraries in a central database are the typical solution. We have a network drive that contains our various .schlib and .pcblibs hat are divided and organized by part types. For instance, you could have something like the following....

Cap.schlib for all capacitor symbols,
Res.schlib for all resistor symbols
IC-D.schlib for all digital IC symbols
IC-A.schlib for all analog IC symbols
Mech.schlib for all mechanical parts (shields, etc.)
etc.

Then you will have separate footprint libraries. Something like the following:

Passives.pcblib for all passive component footprints (resistors/caps/inductors/etc)
IC-SMT.pcblib for the surface mount, non-through hole IC footprints
IC-TH.pcblib for all through-hole ICs
Conn.pcblib for all connectors
Mech.pcblib for mechanical parts
etc.

The library path in the project options would then point to the folder containing all the above libraries on our network drive. As long as the symbol calls out a footprint name that is contained within one of the various pcblibs, the tool will locate the proper footprint. Just make sure you don't have any duplicate footprint names amongst the various footprints. You can force certain libraries, but it's easier to just set it to "any library" and use unique names.

I usually use the integrated libraries solely in cases where the designer does not have access to the complete library files (i.e. remote off-site design). The integrated library only contains the parts used in the current project, so you wouldn't have access to new parts. Also, any changes or updates made to parts within the integrated library would not be directly available for use on other projects. So I suggest sticking with individual .schlib and .pcblib in a central database.

Hopefully that clears somethings up.

Wouldn't it be better to use a parts based library, thus one part would have only one generic footprint (the only alternates being IPC-7351 N or L)...the parts being explicit in that the full part number including package is used, this does prevent errors at the assembly stage.

I obviously don't know the OP's original intent on requiring multiple 3D models for each part, so I described a method to possibly achieve his desired outcome based upon my understanding of what was written. It's something I myself have not required before, and therefore I stick with the standard where each part gets its own symbol and footprint. If a newly added part shares the same basic footprint as a current part (i.e. same pad dimensions, same pastemask, same silk, etc.) but differs in its 3D body (perhaps different vertical height), then I would create a new footprint (with the new 3D body) that would be called out in the new part's symbol. The new part symbol would not include the previous (shorter vertical height) footprint. And likewise the older shorter parts would not include the taller footprint in the symbol.

Just to illustrate a case where it may make sense to have multiple footrints with varying 3D bodies.... For instance, the OP's differences between 3D bodies perhaps may be simply a change in color on the model, which they use at the test stage to indicate the parts purpose. Perhaps a blue connector on the drawing indicates an input signal, and a red connector indicates an output. The actual part placed on the assembly is the same color whether it's an input or an output, but the 3D body drawn in their drawings is color coordinated accordingly. That is a case where adding multiple footprints that vary in 3D body alone might make sense. But just speculating here.