How to make blanket apply rules based on component, not the net - Page 1
Forum section: electronics / general

author: poorchava
author_rank: Super Contributor
timestamp: February 04, 2014, 06:04:54 pm
content: I've recently started using blankets to specify some PCB layout stuff from schematic. In this case I wanted some components (namely: boost converter) to have direct connection to polygons, for the sake of lower inductance, while the rest of the components should have thermals in order to minimize tombstoning.Now I have specified in DRC that in general polygon connect style should be a relief, and i have placed a blanket over the boost controller adding a rule that polygon connect should be direct.For some reason, the rules generated by the blanked turned out to be of "InNet('GND')" kind, which makes other components connected to those networks also have direct connection to GND.Is there a way to tell altium, that I want blankets to create rules based on component, not based on net?

author: AlfBaz
author_rank: Super Contributor
timestamp: February 04, 2014, 06:54:59 pm
content: Can't say that I've used "blankets" yet but have you considered using component classes? If the "boost converter" is on it's own schematic you may be in luck. Open the PCB and under Design->Classes you have a bunch of auto generated Component Classes based on the schematic that contains them. Perhaps this may be a better chioce

author: armandas
author_rank: Frequent Contributor
timestamp: February 04, 2014, 08:57:17 pm
content: +1 for using component classes.For each component that you want to connect directly to the polygon, add a ClassName parameter with some class name (e.g. DirectConnect) as a value.In PCB design rules, specify the direct connect for all components that match InComponentClass('DirectConnect') query.

author: poorchava
author_rank: Super Contributor
timestamp: February 04, 2014, 10:20:51 pm
content: A component class can be easily generated by selecting components on schematic and then in class generator setting 'selected' to true and everything else to 'any'.On the side note, I find it kind of stupid that you cannot attach pcb layout rule markers to components, only to nets. Adding that stuff to each component's properties one by one is cumbersome, and there doesn't seem to be a way to do it from property manager (which it should, IMO)

author: peter.mitchell
author_rank: Super Contributor
timestamp: February 08, 2014, 02:00:03 pm
content: Quote from: poorchava on February 04, 2014, 10:20:51 pmWhat kind if stuff do you want to add to each components properties?If you wish to add a ClassName parameter to a large group of components, you can select all the components and then press F11, this will bring up the inspector, scroll down to where it says add user parameters, type in the desired class name, then in the pop-up window, type ClassName and hit ok.If you want to make it a little easier or "bullet-proof", you can use the find similar tool to select a group of components, and then use the inspector with that selection, EG, to add a class name to all of your caps, you could right click on a cap, click find similar, set type : component/part = same, designator: C* = same, hit OK, and then add the classname in the inspector.

author: mrflibble
author_rank: Super Contributor
timestamp: February 11, 2014, 01:35:15 pm
content: You can combine blankets with net or component classes to get the desired effect. Since I am far too lazy to type all that stuff, take a look at this instead:http://techdocs.altium.com/display/ADOH/Defining+Net+Classes+by+Area+on+a+SchematicThe above describes it for net classes, but you can do the exact same thing for component classes.