altiumfootprintpcbpcb-assemblypcb-design
I am currently trying to use the database in Altium, but I have one big question:
I was expecting to get one database entry per resistor value. But, for a single 100k 0805 resistor (for example), there are three footprint choices, by density:
Why three choices for the footprint? How do I choose?
Making the footprint is generally one of the fastest of all the things you need to do. There are Wizards in Altium that help you make IPC-compliant footprints quickly, and you can set the text height, silk screen line widths and so on to conform to your specific requirements and so your boards have a consistent appearance and set of manufacturing requirements.
Populating the data base with all the things that should be there (vendors, part numbers, alternates, prices, and so on) takes longer. Making a 3D body, if you need to, can take a lot longer depending on your proficiency with 3D parametric modelling software and whether you want to do a good job, a spectacularly good job, or something more slapdash. Here's a rendering of an LED body I did some time ago- the actual die dimensions and position is shown but I didn't bother with the bond wire. The typical library parts often have a crude 3D block or nothing at all.
You only make the part once and you can re-use it thereafter. It's a big hassle to add parts to inventory for the rest of the company, so maybe it will make you think twice about reuse.
Anyway, if you're at the beginner stage (we've all been there) and you just want to get going, use an 0805 resistor and it will be sub-optimal but usable (ignoring the 3D features and such like). You can edit it to show the polarity and save it in a library of your own. You can also download someone else's library that's been done more-or-less properly and (hopefully) learn from that and create your own as you gain experience. IIRC, the 0805 and other Imperial standard footprints may use the metric equivalent numbers (2012 for 0805) as part of their names.
The ideal footprint doesn't just depend on the package size. You should also consider:
The height of the contacts on the part (not all "A size" capacitors are the same, for example)
The mass of the part
Whether you're doing reflow or wave soldering.
For reflow, The thickness of the stencil you'll use.
How much you're willing to trade off assembly defects and reworkability to cram more parts on your board.
So whatever footprints are provided by Altium, they're not likely to be ideal for your design. (And you also shouldn't just blindly trust the footprints provided by the part manufacturer --- they'll give you a good compromise footprint, but not necessarily the best one considering all the details of your design)
But if you're doing hand assembly in low volume, you can probably get away without having the absolute "ideal" footprint. And the provided libraries (at least for common two-terminal devices) are probably acceptable, whichever one you choose.
Best Answer
The IPC Density setting has to do with how tightly-packed with components your design will be. In Altium (and other software) this will affect both the land patterns and also the clearances.
For example, "high density" is to be used if you need to place components very close to each other. A high-density footprint will have smaller soldering locations and also will allow parts to placed closer together without raising any errors.
I would recommend low-density unless you run out of room. The primary reason is for ease-of-soldering. The low-density pads are generally large enough to solder to by hand, whereas the high-density pads can require reflow soldering.
Also, some assembly houses charge a premium for tightly-packed component placement.