Altium Designer - Putting text into a pad. - Page 1
Forum section: electronics / general

author: aouate3
author_rank: Newbie
timestamp: April 18, 2014, 07:56:58 am
content: I have been given the task of putting text into a pad on Altium Designer. Yes I realize that soldering over the pad would make the text unreadable. The reason for putting the text in the pad is for board space. How would I go about doing this? I have attached an image of how my employer wants it to look like.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 18, 2014, 08:44:45 am
content: What kind of text? Take your pick:Negative CopperPositive SoldermaskPositive SilkscreenOr if it's really big, routed board slots/holes?You can pick any (in any compatible combination of layers, e.g., silk "inlaid" over negative copper), but it won't be a "pad", i.e., a single copper object to which a net can be assigned and routed. If you're lucky, the copper (if any) can be connected to a net without DRC (if you can't get that to work, build a footprint and set it as a net bridge object so the unassigned copper doesn't generate DRCs).Tim

author: DerekG
author_rank: Frequent Contributor
timestamp: May 04, 2014, 05:37:49 am
content: Quote from: aouate3 on April 18, 2014, 07:56:58 amYour employer obviously does not have an engineering degree! What is the point? As soon as you wave solder the boards, it will be gone. It could also affect the integrity of the solder joint itself.How about you add the name over the top of the track attached to the pad on the silk screen layer.Actually, what you want is quite easy. Double click on the pad (or single click depending on your Altium version & the preferences you have set up) to select it, then change the pad number for "5V". Example is shown below. This will of course show the pad change when viewed in Altium pcb (for your reference so it replicates the finished product).Then you need to manually manipulate the solder gerber by adding "5V" as a solder mask on the appropriate pad.

author: RoMaNo
author_rank: Newbie
timestamp: May 15, 2014, 04:43:22 am
content: I'm not sure this is the best way to do something like that but there are scripts which allows you to import bitmaps to your PCB. So you can draw this "pad" with Paint (using a black and white bitmap) and then import it using one of these scripts. You can choose the destination layer so it can be part of the silkscreen but also a shape drawn in your top layer.http://techdocs.altium.com/display/ADOH/How+to+import+a+graphic+onto+the+PCB+overlayRemember that if you need exposed copper you must draw the soldermask opening manually.By the way, if you have a very populated area and it is impossible to mark all pads and components with the silkscreen maybe you can draw a map elsewhere.

author: tautech
author_rank: Super Contributor
timestamp: May 15, 2014, 05:18:07 am
content: Quote from: aouate3 on April 18, 2014, 07:56:58 amI saw this was still active and then it dawned on me!Create pad label as bottom layer copper text. Adjust to size needed and place where needed.Create pad as a polygon pour around text using a rule for desired clearance.Assign polygon poured pad to the net required.I would somehow try and copy it to a personal library for future use. Maybe a copy & paste to a PCB file or create a new footprint with enough room inside for the labels needed.It is a bit of shagging around, but it is possible.

author: dsc-pcb
author_rank: Newbie
timestamp: August 07, 2014, 01:59:09 pm
content: I think you can set the the copper layer as negative, then you can add the text as what you described.

author: Batang
author_rank: Regular Contributor
timestamp: October 05, 2014, 06:12:06 pm
content: QuoteAn alternative method of adding logo's etc to the PCB with AD is to create a custom true type font with your logo and then drop it in the windows font folder.On any layer place a string and select your font and appropriate character for your logo etc, you can now control height, width and rotation.Cheers.