How manage footprints for axial resistor vertical or horizontal mount

You could set this up as an Alternate footprint. Switch between the two in layout.  Easy.

CIS duplicate issues notwithstanding, for volume, if you look at assembly, I think you want this to be reflected on the BOM, in case you have leads formed, crimped and put on tape-and-reel...   

And, this orientation change may surprise the mechanical engineers if they are running CFD thermal sims.  But, it's been a while...

Thanks for the heads up - I'll try to follow the directions specified here community.cadence.com/.../dual-footprint

Hi Eddoh

From experience I think you are far better off creating a dedicated footprint for your vertical mount resistor. The advantage here is the pcb symbol name can or a description of what the part is can be reflected in the BOM.

As RFinley pointed out it is possible to use an alternative footprint defined in capture with the ALT_SYMBOLS attribute and that particular footprint can be chosen and used in the layout editor when creating your board.
This works fine but from the perspective of capture, capture will not know the alternate footprint has now become the "primary" footprint used in the layout. It certainly used to be this way, not to sure if 17.4 or 17.2 was
updated to fix this. If it has maybe someone can chime in on the details.

So another shall I say more creative method does exist to handle dual use parts. if your design can stand it, it is certainly possible to have dual use footprints for both Horz & vert mount.

For example. In the schematic we have a resistor symbol & as we all know a resistor has 2 pins which means two pads for the footprint typically. But the thing is in the footprint we basically need 3 drill holes to handle
both the vertical and horizontal footprint and to keep things in concert with the schematic from a net perspective we have to have just 2 pins in our footprint. So how to do that ?.

Take a look at this picture of a standard PTH resistor and for clarity it's 3d view.

So the trick is to make the pad into a pad with 2 drill holes. This gets done when creating the physical padstack. The padstack is using multi drill "Offset to be where you would need the drill holes"

In the 3d view you can see the pins more clearly. Main thing here is that we still actually have 2 pins so electrically it is fine with the 2 pin resistor in the schematic.

So all that glitters is not gold. The disadvantage is that for a radial part you would be using more PCB area as the physical part is still an axial type but if that's not a problem then it would work.
From a BOM perspective you would need a way to show that the part is vertical so the board could be assembled.

This particular example is probably not optimal but certainly do-able. Maybe it may give you some insight to what can be created if in a pinch.

All the best.

Thanks for the info. In terms of representation, using a single three hole footprint does not seem to bring a lot of advantages (space, extra holes and also the stp 3D representation does not look that tidy.

So, if I got everything right, you can manage ALT_SYMBOLS in PCD designer. But there is no way to show alternate footprints in the CIS database explorer, right? 
I mean here

Just to understand if alternate footprints are defined..

The PCB Editor can use alt symbols only if capture passes this info to it. Capture knows nothing about alt symbols other than it is a attribute that can get passed to the PCB Editor.

If ALT_SYMBOLS does not exist in your CIS database then from the perspective of CIS it wont display anything that does not exist.

More than likely ALT_Symbols was never defined in the CIS Database. You may want to verify it is there or not..

BTW. All the CIS database does is make it easier to add properties to the schematic symbol on your schematic by keeping them in a database. In days of old before CIS a engineer would have had to do this manually.

Just because the database does not contain a field does not mean it does not exist in the schematic symbol. You can verify this by placing a CIS resistor on your schematic. Double
click on the resistor which will open it's properties. Sort the filter view by "Cadence Allegro"

Do you see the ALT_SYMBOLS field ?, I am thinking it should be there but has no entry which indicates it wont be used during the netlist phase of the design.