Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
I'm trying to create a footprint for a Molex connector but I don't think it is possible to do with the wizards inside Altium, so I guess I have to do it by hand, but I am completely lost. Any help, tips, tricks, tutorial, video or whatever would help me out. The component wizard has an "Edge Connector" but I think that is something different.
Here is the connector I want to create the footprint for. It's the 3 pin version.
Download the STEP (.stp) model from the Molex web site. Unzip it somewhere sensible. Also open up the datasheet drawing.
Open up your footprint library. Do Tools->New Blank Component.
Since the component is specified in mm in the datasheet, switch to metric units. Press 'O' 'B' to bring up the board options. Switch to metric
Now to place the 3D model. Press 'P' 'B' (for Place Body). Click 'Generic STEP Model', then 'Embed STEP Model' and select the file. Set the X rotation to 90º and the Standoff height to 2.9mm.
Click OK, and place the model on the document. Now drag the purple rectangle by the middle of its lower edge, and snap it to the origin.
Now to place the pads. According to the datasheet, the pads for the connector are 0.85mm x 7.00mm, and are placed 1.50mm apart.
Press 'P' 'P' (for Place Pad), then press 'Tab' to bring up the pad options.
Set the X and Y size of the pad, and make it rectangular. Set the Designator to 1, and the Layer to Top Layer. Click OK.
Now place the three pads on the document. Do the left one first (at -1.5, 3.0), then the middle one (at 0.0, 3.0), then the right one (at 1.5, 3.0). Right click to stop placing pads.
Now press '3' to go into 3D mode. and check that the pads look like they're placed correctly.
Go back into 2D mode '2' to place the silk screen. Switch to the Top Overlay layer, and press 'P' 'L' (for Place Line). Press 'Tab' to set the options, and set it to 0.2mm. Draw in some lines to give an indication of the part size. Don't draw them over the pads.
Now go to Tools->Component Properties. And fill in the properties.
Save the library and you're done.
Follow the link you posted.
Then click through to the PDF sales drawing. In the upper center you'll see the recommended footprint. It's just one rectangular pad for each pin of the connector (I think 3 in your case).
In Altium, create a new footprint. Give it a reasonable name.
Use a 0.5 mm grid to make it easier to place your pads.
Add 3 rectangular pads with the dimensions given in the Molex drawing. Place them in a row spaced 1.5 mm center to center, as shown in the drawing. Make sure they're numbered 1, 2, and 3, in the correct order. You might want to put pin 1 at location 0,0 or you might want to put the middle pin at 0,0, whichever you prefer.
Then draw whatever you want on the silkscreen layer. Probably you want to indicate at least the rough size of the outer housing of the connector to aid in placing other nearby parts. You also want to have something on the silkscreen (like a round dot or a numeral "1") to indicate pin 1. Make sure that the pin 1 indicator will be visible even after the part is placed on the board.
That's pretty much the whole story.
