Dimensioning tools in Altium PCB - Page 1
Forum section: electronics / general

author: rubdub
author_rank: Newbie
timestamp: September 29, 2013, 12:42:53 am
content: Is there any way to dimension pads in the footprint editor of Altium? I'm talking about tools similar to those of mechanical cad packages such as solidworks/autocad.Also, is there any kind of measuring tool to measure the distance between points on a PCB footprint?I'm ripping my hair out trying to create footprints for parts such as usb ports...

author: David_AVD
author_rank: Super Contributor
timestamp: September 29, 2013, 01:40:04 am
content: Doesn't the Report > Measure Distance tool do what you need?

author: rubdub
author_rank: Newbie
timestamp: September 29, 2013, 01:59:25 am
content: Quote from: David_AVD on September 29, 2013, 01:40:04 amYes, that's exactly what I was looking for to measure distances.Is there any tool that can do the relative dimensioning of pads shown in the picture below?

author: David_AVD
author_rank: Super Contributor
timestamp: September 29, 2013, 03:07:02 am
content: I usually create all of the pad objects (at their required dimensions) first, then shuffle them around.It's a real pain when the data sheet has edge to edge dimensions and you're moving the pads by their centre points though.You can also select a pad (or more than one) and then use Move > Selected to drag it via an origin other than the centre of a pad.

author: sacherjj
author_rank: Frequent Contributor
timestamp: October 01, 2013, 11:09:49 am
content: I like to add Guides for positioning: lace -> ork Guide -> ertical or orizontalThis works in PCB and PCBLib.I find that laying out a complex footprint, it is easy to throw some guides up based on the data sheet and then place pads sized right and move into the right location. It is invaluable when doing those odd shaped pads as well. It also keeps you sane when making a PCB trace antenna as a pad or pads.

author: free_electron
author_rank: Super Contributor
timestamp: October 01, 2013, 03:12:35 pm
content: Make sure the i spector panel is open in pcblib. You can change all the criteria of elements there.Seleectt he pads you want to modify and simply change the parameters there.As for precise positioning.I dont bother with guidelines and measuring.Just set the grid to the correct pitch.Look at the bottom. Altium shows you absolute xy coordinates and relative coordinates (like when drawing a trace). I simply draw the traces on a mechanical layer.Lets make a component , 'the free_electron way'To begin we need four pads 1.27 mm apart.I place my first pad somewhere. I dont care where. Just place it.Edit -set origin -pin. And click on the center of the pad. Make sure snap to object centers , and snap to grid is on in the snap control lanel (bottom right of the screen is a little tab that says snap)Now. We have our first pad and the coordinate system is centered on there.G grid. Type in 1.27mm and hit enter.Place three more pads on the grid. Click click click.Now, we need a pad 4mm above these and centered between the middle two of the four we just placed.G grid . 1.27 halved is 0.625 so key in 0.625.E set reference to position. And click on the gridline centered between two middle pads.G 4mmGo one gridline up. Bang place pad.Essentially you use the set origin function to define the starting point and you use the grid function to pick the correct offset. Be ause altium 'snaps' to objects and grids the creation process becomes extremely simple.If you have a step file it is even easier. You go in 3d space, place markers on objects, flick to 2 d mode and you placement will snap to the markers. No measurements required.Leave all the calculations to the machine