Altium PCB component adjustment - arc? - Page 1
Forum section: electronics / general

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: June 25, 2024, 01:15:34 am
content: Hello Experts,It's my dumbass again. I need some guidance on how to fix an annoying PCB quality of life issues.I do not know proper terminology, but I have several test points that are no longer centered on what Altium expects the component to be. Please see attached snip. I need to click on the larger 'pad' to move the test point.1. What is the proper terminology for this? pad? polygon?2. When prepping the Job Output and selecting which properties to print to PDF, toggling 'Arc' would show it to print or not, so that is what I was looking for using Google-Fu.3. How can I fix such a seemingly simple thing without deleting and then updating the PCB project file?

author: free_electron
author_rank: Super Contributor
timestamp: June 25, 2024, 01:35:10 am
content: did you unlock the primitives by accident ?right click the component ( not the pad, the component itself. if you can't grab it : turn of everything but components in the selection filter) then select component actions -> reload from library. that will restore it

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: June 25, 2024, 05:46:12 pm
content: I will try that and follow up.I think Altium has their own help forum, so I will post there that way I will not clutter this forum with inane posts.

author: ajb
author_rank: Super Contributor
timestamp: June 25, 2024, 06:44:11 pm
content: The green circle thing in your photo that says "VCC" in the middle is a pad -- it defines the hole and the physical copper pads that form the connection to the component. The hatched rectangle looks like the 3D body for the test point, and it looks like there is a circle (in Altium, a circle is a variant of an arc primitive) on the silkscreen as well as maybe another one on another layer (courtyard?).Is there only one of those test points that has this problem? free_electron's suggestions should work, or you might be able to delete the component from the PCB, then update from schematics to get the component back, and just move it back into position.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 25, 2024, 09:12:51 pm
content: You can always find out what an object is by selecting it in PCB view and opening the Properties (older versions, Inspector) panel or dialog. Type is at the top.If it's a footprint, the objects it's made of are locked by default. They can still be selected with a query (open Query panel, run something likeInComponent('TP_VCC') and IsArc and OnSilkscreen, or other component-identification, object-type or layer-selection terms), or the component can be set to Lock Primitives = False (which may be how this happened). If it's not a footprint, consider selecting the objects and assigning them to a Union, so that dragging any one object tends to drag them all (you can still M, S (Move Selection) or CTRL+arrows to move a selection independently).Tim

author: exmadscientist
author_rank: Frequent Contributor
timestamp: June 26, 2024, 08:03:26 pm
content: So what has probably happened here is related to a change Altium made around version 21 or so. Before that, a component's bounding box was defined by Altium making up something related to the largest rectangle that could enclose all the component's pieces. After their change, the bounding box is defined by whatever's on the Courtyard layer. Primitives within the component retain their own selection areas.This is usually pretty sensible... but doesn't work out so well for test pads. If you define the Courtyard to be a fairly tight circle around the pad (as works pretty well for these guys in meat-space), it will besmallerthan the bounding box for the actual testpad, the copper bit. So when you click on the dumb thing to move it around, you're very likely to move the pad (just the copper piece) instead of the test component (the whole lot including the pad, silkscreen, any 3D, etc.).This is kind of annoying. It would be fine except that for whatever reason, Altium tends to like to detach the pads from the components sometimes, as if primitives were unlocked. I haven't quite figured out why or how it happens. So you end up with the pad in a different place than its markings and its officially recorded location. Not good.This bit me on a design I did recently and would have seriously screwed up the test fixture, for want of one pad being off... fortunately, for not-my-fault reasons (promise!), we needed another spin on that one and I got to slip in a fix

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: June 27, 2024, 07:43:16 pm
content: Quote from: exmadscientist on June 26, 2024, 08:03:26 pmIn the spirit of following up, I think you are correct. I inadvertently made a change to (I presume - sorry, still new to the tool) the pad and other primitives. The via (pad?) I changed the X-Y coordinates causing that offset.

author: tooki
author_rank: Super Contributor
timestamp: June 27, 2024, 08:08:53 pm
content: Quote from: ajb on June 25, 2024, 06:44:11 pmThere’s no need to delete it and move it back — you can just take the component and update it from the footprint. In that process, it gives the option to fully replace it. You can also do this from the schematic library.