How to disable thermals in localized GND pours? - Page 1
Forum section: electronics / general

author: senso
author_rank: Frequent Contributor
timestamp: February 13, 2015, 02:56:17 pm
content: Good evening, so here I am playing around with Altium and I'm sort of starting to understand a little bit more of the Query system, and I can in fact have pours with and without thermals, different sizes and what not, but only if the pour is connect to some net that is NOT ground, here is what I want to do:I have already tried using InNamedPolygon, InPolygon and some other random things but the GND vias always have the thermals enabled, yes I have tried changing the Priorities, and putting the rule in either the Polygon Connect Style and in the Power Plane Connect Style, is there something I'm missing/failling to understand(it must be me, of course).Care to enlighten me?Best regards.

author: ajb
author_rank: Super Contributor
timestamp: February 13, 2015, 07:57:00 pm
content: You can get all vias to direct connect by using IsVia, would that work for you? Simpler than having to name polygons.

author: free_electron
author_rank: Super Contributor
timestamp: February 13, 2015, 08:20:38 pm
content: write a ruleif isvia and innamedpolygon 'blabla' -> directconnect

author: senso
author_rank: Frequent Contributor
timestamp: February 13, 2015, 08:21:40 pm
content: The isVia works, but it would remove thermals in all the vias, maybe not a bad thing and in this situation can work, but I would like to know how to do it using named polygons, its a more powerful/flexible option in my view.I will try that Free_electron.

author: free_electron
author_rank: Super Contributor
timestamp: February 13, 2015, 08:41:32 pm
content: oopsie i made a mistake you need IsNamedPolygon , not InNamedPolygon.we are not testing if we belong to the polygon (In...), we are testing if we connect to (Is)so :Make a polygon style Rule :Where the first object matches - Advanced - isviaWhere the second object matched , advanced - Isnamedpolygon('blabla')Connect style - direct connectdon't forget to increase its priority to sit above other rules ( bottom left of window : increase prorities and shove this rule to the the top.i just tried it . works flawless.if you have more than one polygon you can alter the 'where the second object matches toIsnamedpolgon('firsrone') or Isnamedpolgon('secondone')and so onor you could make a polygon class and simply test against the class.

author: ajb
author_rank: Super Contributor
timestamp: February 13, 2015, 09:20:31 pm
content: Speaking of understanding the query system, as you start to do more advanced queries, you should be aware that operator precedence may not be as you'd expect, and as far as I know is undocumented. So to be on the safe side, use brackets wherever there may be any ambiguity to ensure that the query is evaluated the way you intend--that can save you a lot of frustration!

author: free_electron
author_rank: Super Contributor
timestamp: February 13, 2015, 10:02:37 pm
content: i always use brackets. even in maths. for two reasons :1) i can never remember what goes first2) i can't be bothered to try to learn what goes firsthas kept me out of trouble all my life.

author: senso
author_rank: Frequent Contributor
timestamp: February 13, 2015, 10:42:47 pm
content: Just tried it, works perfectly, I was also doing it for other nets/polygons and I was doing it a little different, I had All in the second part of the query, it worked, but now I understand the beast a tiny bit better.Thanks for the help Free_electron and AJB.

author: free_electron
author_rank: Super Contributor
timestamp: February 13, 2015, 11:49:46 pm
content: Quote from: senso on February 13, 2015, 10:42:47 pmi f you really want to unleash the full power of Altium : dig into filter expressions and manipulating the SCH list and PCB list viewers. Then hop into writing scripts. you can make this monster do amazing tricks.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 14, 2015, 04:38:24 am
content: Quote from: free_electron on February 13, 2015, 11:49:46 pmI was comparing a new schematic (captured by hand from a customer PDF) to the bill of materials, earlier today. This involves a combination of filtering, sorting in the List, selecting the components you're checking, and comparing that listing to the spreadsheet -- say by copy+pasting the column into the spreadsheet and comparing the list, element by element, to see that they match up. Which checks that you know you have the right designators, and the right number of them. Then, since the listings line up, you can add the attributes wholesale to the components in the schematic with a single paste operation. A pain to set up, but very powerful.Also, once you have that part list, filtering it again is easy: make a column beside the designators that formats it as "(Name = '<refdes>') OR", repeat for all <refdes>, copy the column and paste it in the filter box. After a few seconds of thinking, Altium determines your selection / mask....Afraid I don't have much to contribute to the thread, as it's already been answered...I will add my preference though: I merely assign all via-in-poly as direct. As far as I know, the only downside to this approach is making them difficult to solder, if you should ever need to add a jumper/bodge wire to one. However, I also put accessible test points (which do form thermals) on all nets (near 100% nodal coverage), so I doubt that it's a big deal.I also like to tent vias-in-poly, since it looks sexier. However, it is helpful to keep a few open, rather than tenting all of them, in case you need additional "accidental test points" shall we say.Tim

author: 74HC04
author_rank: Contributor
timestamp: September 26, 2017, 10:31:22 am
content: Quote from: free_electron on February 13, 2015, 08:41:32 pmThank you very much for posting this, free_electron. You just saved me from pulling my hair out!