Footprint in Altium Designer - Page 1
Forum section: electronics / general

author: nsh1233
author_rank: Contributor
timestamp: July 08, 2014, 05:42:57 am
content: Hello!I'm trying to make a footprint of a LED (HSMH-C190.) for my project and i'm confused which dimension in the datasheet do i use? There is the package dimension and a reccomended soldering pattern.And for the footprint of the LED, is making just the pads sufficient? or do i need to draw the overlay, net, green cross like the resistors and capacitors?

author: David_AVD
author_rank: Super Contributor
timestamp: July 08, 2014, 06:08:27 am
content: At the minimum you'd create the pads using the recommended pattern. How much else you draw is up to you. I tend to draw the overlay and add a 3D model for almost everything these days.

author: sacherjj
author_rank: Frequent Contributor
timestamp: July 08, 2014, 11:32:18 am
content: It is also a good thing to standardize on what mechanical layers you will use for things early and build the library with that.This is from my docs that I made for standardization. Most of these are Altium defaults. If you draw the M13 body layer for a component, then you get an automated assembly diagram, with a little moving the part reference around. This is very handy to give to your board assembler.Mechanical 1 (M1) ?BOARD OUTLINE ?Board Outline?Mechanical 2 (M2) PCB INFO ?PCB Info (manufacturing info added as text)?Mechanical 3 (M3) FAB NOTES ?Fabrication Notes (for PCB producer)?Mechanical 4 (M4) ?PANEL NOTES ?Panelization Info (V-groove and tab locations, etc)?Mechanical 5 ??Mechanical 6 ? ??Mechanical 7 ??Mechanical 8 ??Mechanical 9 ??Mechanical 10 ??Mechanical 11 (M11) TOP DIMS Top layer dimensions (paired with M12)?Mechanical 12 (M12) BOTTOM DIMS Bottom layer dimensions (paired with M11)?Mechanical 13 (M13) TOP BODY ?Top layer component body information (3D models and mechanical outlines, paired with M14)??Mechanical 14 (M14) BOTTOM BODY Bottom layer component body information (3D models and mechanical outlines, paired with M13)??Mechanical 15 (M15) TOP ASSY Top layer courtyard and assembly information (paired with M16)?Mechanical 16 (M16) BOTTOM ASSY ?Bottom layer courtyard and assembly information (paired with M15)

author: twistedresistor
author_rank: Contributor
timestamp: July 09, 2014, 01:29:49 pm
content: Hi nsh1233,in theory the pads are sufficient to function, but you should add a few extra infos.You should at least add information about the physical size and the silkscreen for your part.You used the IPC Footprint wizard? The layers used there can be referenced as a semi-standard for usage of the mechanical layers.As a bare minimum besides the Pads add:- the outline of your physical component (M13), for reference to not place other parts too close- the silkscreen (top overlay) for the markings on your PCB- for flavor you can add a 3d representation of your component (also M13)HTHtwistedresistor

author: sacherjj
author_rank: Frequent Contributor
timestamp: July 09, 2014, 03:18:20 pm
content: Quote from: twistedresistor on July 09, 2014, 01:29:49 pmI put the outline of the physical component on 15, which is Altium standard. The 3d on 13. This makes layers 15 and 16 the assembly diagram (top/bottom).

author: nsh1233
author_rank: Contributor
timestamp: July 10, 2014, 01:00:38 am
content: Thanks everyone!Quote from: twistedresistor on July 09, 2014, 01:29:49 pmCan i use the top overlay to draw the outline of my component?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 10, 2014, 10:58:16 am
content: No, overlay is only printed over soldermask. PCB manufacturers almost always cut silk over exposed copper pads.I normally draw the 3D outline (usually as a body on Mech 13) based on the "typical" dimensions in the datasheet. Silk, I draw the same outline oversized by one grid space (0.1/0.2 mm, or 5/10 mil, as appropriate to the part), over what places it can be drawn -- a chip resistor gets only two parallel lines, truncated by the pads (or if the pads are very close together, a single line segment down the middle). I try to use a silk outline representative of the component outline (say, if it has bumps and knobs sticking out), and include some notable features (e.g., the inner profile of a connector, or polarizing marks). I use Mech 1 for the center coordinate (a small cross; I think Altium defaults this to Mech 15), and draw the courtyard rectangle (on Mech 15) one grid space oversized from any silk, 3D or copper feature (so, for devices with profiles smaller than their pads -- chip resistors, SOICs, etc., the edge of the line is touching the edge of the pads; or bounding the silk outline for components that span their footprints, e.g., radial TH electrolytics).STEP models are preferred where available, otherwise, 3D primitives until it looks kinda-sorta correct (body, housing, pins, etc.). 3D data is added whenever possible. No extra marks on other layers, labels, etc. Only good looking things.Speaking of labels, and other layers, on the PCB, I usually hide the name of non-populated test points, show comments of most wires and connectors, and for mechanical features (holes, fiducials), move the name to Drill Drawing so they are identified on the mechanical outline.Tim

author: sacherjj
author_rank: Frequent Contributor
timestamp: July 10, 2014, 07:51:32 pm
content: Many component makes have downloadable STEP files and I've found it very worthwhile for strange or complex footprints as a way of validating my pad size, shape and location. Then, you get great board renders for free.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 10, 2014, 10:59:27 pm
content: Except for the ones that are all whiteTim

author: sacherjj
author_rank: Frequent Contributor
timestamp: July 11, 2014, 11:40:17 pm
content: Quote from: T3sl4co1l on July 10, 2014, 10:59:27 pmI've got a microSD model that they decided SD cards are neon green and the holders are purple.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 12, 2014, 01:33:50 am
content: Recently saw one encoder (vertical, PC mount, potentiometer style) where the model showed oranges and blues and all sorts of whacky inappropriate colors...Tim

author: twistedresistor
author_rank: Contributor
timestamp: July 15, 2014, 08:41:46 am
content: Quote from: sacherjj on July 09, 2014, 03:18:20 pmNo, layer 15 is the courtyard and not the physical outline. The physical outline should go on 13 if you want to adhere to the FP-Wizard standard.The courtyard is bigger than your overall component, including the pads. (e.g. for a chip resistor the courtyard is the component itself plus its pads and this plus a "courtyard access" of 0,25 mm, for nominal density/IPC Level B) The courtyard helps you placing the component to keep it "manufacturable". Basically said, if you place components courtyard on courtyard, it is likely that you will have no problems with shorts and so on when soldering.So if you only put the component itself on the courtyard then you might place your components too closely together. Of course you can define that layer 15 is YOUR layer for the assembly, but it is not the equivalent of the courtyard, and should be kept separate.