I am going to be doing a board that was 6 layers and components are on layers 1 and 5. There is a step down in an area that allows the parts to be able to be mounted to the 5th layer. My question is how to get PADS to mount a component on layer 5?
I've never seen options for mounting parts other than Top and Bottom (layers 1 and 6 in your case). It sounds like you'll have to swap layers 5 and 6 during your fabrication. Or are you mounting parts on layers 1, 5, and 6? That may be beyond PADS capabilities.
Not something PADS would normally handle.
You obviously have to build a custom part.
Build your part normally (like with silk on top or top silk, soldermask, solderpaste, etc). If any pads need to appear on the surface layer, they will be built normally.
For the layer 5 pads, do not put them on Layer 2 in your decal, put them on layer 5, make the mounted side pads of those pads 0 or 1. It actually doesn't matter what size you'll make the surface pads, they're going away anyway, but sometimes PADS will gripe if you make them 0...
If TH, add the other pads normally, if SMT, just have the Layer 5 pads. You will be able to route to/from the Layer 5 pads as if they were on the surface.
Put a properly sized and placed routing/copper, etc keepout on the Decal for the mounted side so you won't get pour or routing or vias or whatever in the cutout area.
You'll have to add a detail to your Fab Dwg for the cutout area, and maybe some additional notes explaining what's happening, but it should work.
Understand that the part will be listed as being on the Secondary (aka Bottom) side, not on Layer 5, in your pick and place file. So that will probably need to be noted for your assembler.
The parts were SM so it was somewhat easy to accomplish. On the final design the parts were placed on layer 1, 2 and 6. Because the parts in the step down area could not have silk screen or solder mask I just had to make custom parts with pads. The fabrication and assembly drawings took a little bit of an effort. Thank for the feedback.
This is unusual pcb design of having components placed on the internal layer.
Even the Pads or any pcb software like Allegro doesn't normally handle this kind of pcb design because
i think it's not a common pcb designing practice unless it's really needed and no other option to choose with.
Just be careful in choosing parts to be placed in the step down area, stripline is not allowed in this area
while microstrip can placed possibly provided if your bottom plane is ground plane.Consider also the parts'
height and weight since there's is a reduction in pcb thickness in that area, SMDs are well suited in this case.
Build your custom part on Pads PCB Decal Editor with pads on layer 5 of the corresponding pcb decal for SMD .
Other properties of the custom part are the same as that of normal parts have. In placing the custom part, it's still at the
bottom side but routing to/from that part is on layer 5 with the aid of vias.
Although you are a Pads user, you may wish to contact your Mentor sales representative and check into the Expedition PCB tool.
If these types of designs will become common place in your line of business, then Expedition is the tool for you
Expedition has the ability to make "Any Mount" parts that can be easily pushed internally into a pcb stack, and with the Embedded Passives and Advanced Packaging capabilities, you can use Embedded Material discretes and cavity designs with ease. Yes, it is true, "Other design tools like Allegro do not normally handle this" - But Expedition Does!!! And very easily!!!
For more info:
Retrieving data ...