Allowing either through-hole or SMD for a part - Page 1
Forum section: electronics / general

author: ledtester
author_rank: Super Contributor
timestamp: September 18, 2025, 11:34:58 pm
content: Suppose you have a part on a board which you want to be able to be populated either with a through-hole or SMD variant.How do you manage that part in your schematic?You could, of course, just put the through-hole and SMD part in parallel and each has their own designator. The schematic might be confusing at first unless you add some comments about what is going on. And how is that reflected in your BOM?Does your layout program have any features which help in this situation?

author: langwadt
author_rank: Super Contributor
timestamp: September 18, 2025, 11:44:23 pm
content: just put both parts in the schematic and make on of them NP/NM/DNP

author: UnijunctionTransistor
author_rank: Frequent Contributor
timestamp: September 18, 2025, 11:51:04 pm
content: I have done that, once, in EasyEdaWhat I did, and I know this method can be improved, is to add both in parallel and distinguish them with a suffix either A or B like U5A, U5B.And add a note to indicate which suffix corresponds to which footprint.

author: abeyer
author_rank: Frequent Contributor
timestamp: September 19, 2025, 03:48:31 am
content: Why do youwantit in your schematic? Shouldn't this be a board thing implemented in the footprint, and not in the schematic at all?

author: PGPG
author_rank: Frequent Contributor
timestamp: September 19, 2025, 07:31:37 am
content: Because of Covid supply problems I had to allow for assembling IC in one of two SMD packages (bigger and smaller). I have made footprint consisting of both this footprints (one inside the other).

author: langwadt
author_rank: Super Contributor
timestamp: September 19, 2025, 10:06:15 am
content: Quote from: abeyer on September 19, 2025, 03:48:31 amthen you need a custom footprint, an I have seen atleast one IC where different packages have different pin numbering

author: w42i
author_rank: Contributor
timestamp: September 19, 2025, 10:49:42 am
content: Yes, it gets more complicated if the SMD and THT pinouts differ.For Rs and Cs I like to use mixed footprints allowing for multiple SMD sizes and THT components to be populated, see the attached image. I use this primarily for precision parts that need some testing.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: September 19, 2025, 06:59:13 pm
content: Best approach for this will be dependent on the software you use.I only have (current) experience with KiCad, and modifying the footprint would be my first choice. You start with a (copy of) footprint "A", and then you import footprint "B" in the first footprint. Relative positions of the footprint can be arbitrary, as long as it does not create shorts and such, but further cleanup is probably a good idea (adjust silkscreen and such). When such a combined footprint is placed on the PCB, then KiCad assumes that pads with the same pad number have to be connected, so it just adds all the pads to the netlist.And as w42i wrote, you have to be careful about pinout changes in between those two footprints. KiCad does not have an extra mapping layer, so you have to modify the pad mapping in the footprint so the electrical connections work with the schematic symbol. (Atmega328 is an example of changing pin mapping with package name).I once also tried the other obvious approach, and put two RS485 drivers in parallel on the schematic. This looks extremely confusing and eats up your canvas space (Especially with bigger and more complex IC's. Imagine all the extra wiring.) In newer KiCad versions you can add "Do not Place" attribute for one of the footprints, but in my old KiCad version, ERC was not happy about output pins shorting with each other.And yet another aspect is the BOM management and the part placement file.

author: Smokey
author_rank: Super Contributor
timestamp: September 19, 2025, 08:39:23 pm
content: I've done this dual pattern thing before, but it's usually for connectors.For Rs and Cs I would do something like this:Where the library part is the dual pattern as shown with both SMT pads and through holes and the "A" and "B" silk.On the BOM you list the part used in those refdes locations. You could even have some be through hole and some SMT as long as they are different line items.In the BOM line item notes, just to make it absolutely clear to the assembly shop, put something like "these component locations are through hole and use "B" pads", or "these component locations are SMT and use "A" pads". It should be obvious based on the type of component listed on the BOM for that line, but since you are trying to be tricky and this is non-standard, just make it super specific in the note.