Disconnecting a inter layer from a multi layer pin - Page 1
Forum section: electronics / general

author: BocaDev
author_rank: Contributor
timestamp: June 05, 2018, 01:54:49 am
content: I was given a Altium PcbDoc file along with the users footprint library to make a modification. No schematic was provided so I have to do manual edits to the PCB board. I am using Altium Designer, Winter 09 (old stuff).Question, there is a transistor with it's collector connected to one of the internal layers of a four layer board. I need to disconnect that pin from the internal layer and then run a track to another point on the bottom layer. How do I proceed to isolate that pin from that internal layer using a manual edit.Thanks

author: AlfBaz
author_rank: Super Contributor
timestamp: June 05, 2018, 02:04:11 am
content: Assuming a) there's a netlist attached to the pcb document and b) the internal layer is a different net to the new connection point then you should be able to double click the pad and in the pads properties change the net it's connected to

author: BocaDev
author_rank: Contributor
timestamp: June 05, 2018, 02:27:12 am
content: Hi AlfBaz,I went into the "all net classes". Then I went down thru every net and removed any connection to that transistors pin. For some reason when I start laying track on the bottom layer, it's giving a DRC error as being shorted to that same internal layer. But looking at the internal plane layer and zooming in, no connection is visible. I guess electrically it will be OK but the error is still showing on the DRC check.Thanks

author: D3f1ant
author_rank: Frequent Contributor
timestamp: June 05, 2018, 05:44:06 am
content: If your going to ignore the error, be sure to check the Gerber very carefully before submitting for manufacture.Editing the pad and changing the net would be safer and easier than trying to edit the netlists manually.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 05, 2018, 07:07:14 am
content: Plane or polygon inner layer?In either case, easiest is to block connection with an object.For planes, place a circle around the pad, so it becomes disconnected. (Planes are drawn in negative space.)For polygons, place a Polygon Cutout Region around the pad.This is purely graphical and will not solve netlist errors.The preferred method is to remove the pad from the one net, and add it to the other net.Don't forget to repour polygons (T, G, A) if you don't have auto-repour turned on (still a good habit even if you do), or rebuild planes if they're in use.If the design is pathological (e.g., inner layer poured with a Region), edit the object's vertices to add a hole around the pin in question, or just delete the fucking thing and place a new polygon in the same outline. This is, uh, hopefully, very unlikely to have been done by a human, but sometimes, imported files create such horrors as this, and you should clean them up.Tim

author: BocaDev
author_rank: Contributor
timestamp: June 05, 2018, 01:18:57 pm
content: Thank you guys, what great stuff!I took the suggestion Tim gave and move the device to another location. I don't mine these jobs created by someone else, but with the schematic file missing, yuk. I like the idea of pushing everything from the schematic.Thanks again to D3f1ant and Tim.