Large X mark on plane layer vias - Page 1
Forum section: electronics / general

author: marshallh
author_rank: Unknown
timestamp: February 03, 2013, 05:55:20 am
content: Every via connected to my GND plane layer has a big green X over it.I thought this was the mechanical layer but that doesn't seem to be the case.Also, is there a way to drag a VIA and its routed traces along with it? Right now I have to rip up the surrounding traces and re-route them if I move the via.

author: free_electron
author_rank: Super Contributor
timestamp: February 03, 2013, 07:00:40 am
content: The cross tells you it is connected trough a thermal on an inner layer.the size of that x tells you what the thermal looks like. these are computer generated and controlled by design rules ( D-R ) and look for 'plane via style'. you can set spoke widht ,clearance and more stuff.if you want to see them : O-L and turn on the inner layers , then, on the top of the layer options go to the right tab( options) and look for 'transparent layers' turn that on.close window.on the pcb editor layer tabs : select the ground plane and you will now get to see what the wagonwheels looks like. you can also turn off all layers apart form the ground or power layer. keep in mind that these layers are drawn in NEGATIVE . anything background color is COPPER, anything layer color is ISOLATION.before fabbing a board you may want to look that there is no overlap on the wagonwheels. actually altium has a DRC rule that can check for that. something called 'orphaned fills' i believe.As for moving the via with the drag : M-D ( move - drag ) clock on the via , if you get a popup box select the via. Altium will try to follow you. it is possible that you need to set an option in the Global menu. Don't remember.make sure that your 'Moses' function is active. ( like Moses going through the red-sea ) shift-R toggles through the modes but it needs to be enabled in O-P ( options preferences) PCB layout tab and check for 'obstacle avoidance' . it should be set to 'push'.

author: marshallh
author_rank: Unknown
timestamp: February 03, 2013, 07:26:52 am
content: Thanks, just what i needed to know. I had turned off the plane via isolation (wagon wheels). Good idea to have it on?Move/drag seems to depend on what is nearby. I played with the obstacle avoidance settings but anytime there are surrounding traces it completely loses its marbles. Will probably just keep manually moving the via and moving the routes manually.Pic shows dragging LDQM down a bit, it correct adds conencting traces but doesnt move the originals. This related to loop deletion?

author: free_electron
author_rank: Super Contributor
timestamp: February 03, 2013, 08:17:17 pm
content: Quote from: marshallh on February 03, 2013, 07:26:52 amthe wagon wheels are a must ... prevents via burnout during plating.loop deletion should not throw a spanner in the mix. ( turn it on ! )what are you trying to do ? you may be going the wrong way and the tool doesn't 'understand' what you want to do. the software is generally very clever , but you have to work inside its range of understanding.there are many things that people try to do the 'hard way' and the tool 'fights'. once you do it the 'right' way ( so the tools 'understands' what the intent is then all of a sudden it works.sometimes it is a matter of invoking a slightly different command. dragging the via is just that : the tool will help you drag the via. if it's about lenght balancing you need to tell the tool : i want to move the via because of length balancing , then it will change its behavior accordingly.are you trying to do auto-lenght balancing ? looking at the snakes in your layout i'd say yes...don't move the via yourself then. leave it where it is. there is an option in the snaking setup that allows altium to pus via's as well. ( be default it only works between pads/via's )don't know off the top of my head where it sits but i believe it is in the preference / pcb/ interactive routing.i think they have a video on the wiki.