Altium - Custom pads creating short circuit violation - Page 1
Forum section: electronics / general

author: martin1454
author_rank: Regular Contributor
timestamp: November 08, 2017, 09:54:54 am
content: Greetings!Im in the middle of an Altium PCB project, where I have created my first "custom pad" for an footprint.I have made an polygon region as the "pad" and placed another pad on top of it, to give it an designator - The design looks about right, but when I use it in my design, I get short circuit between pad and polyregion error.What do I need to change, to let altium know that the polygon region should be a part of the pad?

author: Psi
author_rank: Super Contributor
timestamp: November 08, 2017, 10:47:12 am
content: It needs to have the same designator as the pad its connected to.Looking at your region it seems to have a option for a "Net" but no "Designator"i think you are trying to use the wrong type of region.Have a look for other types and see if you can find one with a designator option.Somewhere in the menu system is an option to convert regions to other types. See if any of those work.'Region' to 'Polygon Region' maybe, im not at my computer to check

author: martin1454
author_rank: Regular Contributor
timestamp: November 08, 2017, 11:39:58 am
content: Looking at the video Altium made, they made the pad by using outline to convert to polygon regionhttp://www.altium.com/video-creating-custom-pad-shapesI have done the same as the video, so I dont think it is the wrong polygon type

author: enz
author_rank: Regular Contributor
timestamp: November 08, 2017, 01:20:42 pm
content: I think you need the Feature "Design/Netlist/Update Free Primitives From Component Pads"This should remove the error.As far as I know, this command assigns the polygon to the net the pad is connected to.

author: martin1454
author_rank: Regular Contributor
timestamp: November 08, 2017, 02:55:32 pm
content: Have tried it - still not working

author: Mikekoz13
author_rank: Contributor
timestamp: November 09, 2017, 11:43:17 am
content: It's probably a rules violation. Make sure that you have "Different Nets Only" selected in your clearance rules.See the attachment.

author: martin1454
author_rank: Regular Contributor
timestamp: November 10, 2017, 08:45:08 am
content: I have "diffrent nets only " selected

author: Mikekoz13
author_rank: Contributor
timestamp: November 10, 2017, 12:23:42 pm
content: Quote from: martin1454 on November 08, 2017, 11:39:58 amI just use "Place > Solid Region" when creating the larger pad that lays over the smaller pad.

author: Mikekoz13
author_rank: Contributor
timestamp: November 10, 2017, 12:26:43 pm
content: Quote from: martin1454 on November 10, 2017, 08:45:08 amTry selecting the "Advanced" button and make sure that "Different Nets Only" is still selected.The other thing to check.... in your Rules is priorities. Is the rule that checks this high enough up in the Priorities?

author: martin1454
author_rank: Regular Contributor
timestamp: November 10, 2017, 12:37:54 pm
content: Think I have found one new thing about it - It is only the pads that have not been assigned to an net (No connect pads)What rule should I look into there?

author: travisc
author_rank: Newbie
timestamp: November 12, 2017, 09:56:43 pm
content: I had the exact same problem. Check out this blog post.https://altiumpcbdesigner.blogspot.ca/2015/07/short-circuit-rules.html?m=1

author: martin1454
author_rank: Regular Contributor
timestamp: November 13, 2017, 08:59:17 am
content: Thank you so much! - That was the solution

author: MT_rel
author_rank: Newbie
timestamp: April 16, 2019, 09:44:36 am
content: I would not agree to create any rule for allowing short circuits, this is a gateway for evil. I have the same issue with Altium 17.1. I have created a footprint in the same way as author of this topic (by Altium recommendations) and using it. Some of the footprints of the same type causes short circuit but other don't. The way I got rid away these problems is to open a footprint in PCBlib editor, change it in some minor way (for example move some copper by 0.01mil), save the library (ctrl+S), then update problematic footprint from PCB library in PCB editor (Tools->Update From PCB Libraries...). And no further violations appears. It seems a software bug for me. One more thing is to keep dimensions of the pad as small as possible with respect to copper region, otherwise custom pad shape will not be recognized as pad. I am using a round shaped pad of 0.1 x 0.1 mm on top on 0.8 x 0.8 mm poly region.

author: ajkahl
author_rank: Newbie
timestamp: May 21, 2019, 05:20:17 am
content: Definitely agree there's a bug here, I can use the same process within the same footprint for multiple pads, when placed on a PCB some pads error, some don't. A non-core change in the library and an "update footprint" usually clears the issue.

author: free_electron
author_rank: Super Contributor
timestamp: May 30, 2019, 06:03:09 pm
content: this kind of thing happens when you load parts after reading in the netlist.DNU will solve that issue ( just type DNU ( design -> netlist ->update free primitives from pads. )for pins that have nothing connected to them it will still be a problem , unless you have the 'create single pin nets' turned on in the netlister

author: dodonny
author_rank: Newbie
timestamp: March 15, 2020, 05:04:40 pm
content: The ast solution was the good one.I got solid region inside my footprint (because you cannot create anything else in footprint) but because you cannot assign any net to those regions... anyway thanks a lot !