Can you define track width in the schematic? - Page 1
Forum section: electronics / general

author: Mattylad
author_rank: Regular Contributor
timestamp: February 10, 2017, 08:48:35 am
content: HI, I have used CADSTAR for many years and am now learning Altium.One thing that is puzzling me is that online tutorials etc. do not seem to be mentioning track width in the schematic at all.In CADSTAR we assign the width of the track (and all allowed widths for it) in the schematic as the schematic is considered the master design document, this then transfers to the PCB and you can start routing once placed, the tracks are drawn in the width decided in the scm.Can and does this happen in Altium?How is it normally done?Cheers,Matt

author: Ice-Tea
author_rank: Super Contributor
timestamp: February 10, 2017, 09:02:13 am
content: This can be done with rules. You can assign a rule in the schematics that assigns a signal to a class and in the rules you can define a width (per layer if you want) to that class.

author: ajb
author_rank: Super Contributor
timestamp: February 10, 2017, 12:23:23 pm
content: You want what Altium calls a "Directive" object. You can attach these to individual wires to affect the relevant net, or you can use a blanket to affect all of the nets on wires in a defined area of the schematic.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 10, 2017, 07:06:31 pm
content: ^ What they said.Be careful applying rules to very general nets, like GND or VCC. You might need a very fine minimum trace width (0.25mm or less) to connect to SMT components, yet a very large minimum trace width in certain places to ensure adequate current capacity. If you want to be very specific about setting width, you'll have to divide the net into sub-nets, joined with net ties (Altium has a way of doing net ties, search for documentation), or zero-ohm resistors or jumpers or whatever. (Or maybe you'll take the opportunity to make the design a bit more mindful, using fusible resistors to supply isolated sections, or using RC or LC filters for them, as is commonly seen in RF circuitry.) The downside is, by breaking it into sub-nets, you've removed that freedom from the PCB designer.You can also use Net Classes, which are less specific (net class rules have to be defined in the PCB, but you can leave a note to that effect in the schematic), but can be applied cleaner (one PCB rule applies to whatever nets are in the class; whereas rule directives create a rule for each net, which gets messy).On a related subject, there are also Pad Classes, which are defined entirely on the PCB. This is useful for selecting specific pads to apply special-case rules to, like to widen or disable thermal relief on pads meant for heatsinking.Tim

author: Mattylad
author_rank: Regular Contributor
timestamp: February 11, 2017, 09:20:39 am
content: OK cheers all.Now I know what area to look in.

author: JamesH-AltiumOfficial
author_rank: Contributor
timestamp: February 20, 2017, 05:44:31 am
content: Hi Mattylad,I noticed your question and dug up an article about this topic, please see below.There are several approaches to defining rules from schematic. The most common way is to just define net classes and then define the specific rules for each class within the PCB document. This way the PCB designer can specify the exact rules for width, clearance, without having to go back to the schematic each time.Place a Net Class directive and attach it to a net on the schematic, then modify it:- The Name is seen on the schematic but isn't transferred so give it a name (or leave as Net Class).- The parameter has a special name called ClassName. Change the value from Undefined to the name of the Class you want in PCB, e.g. Power.- Click OKCopy the directive and paste it on each other net you'd like to be included in the same net class.(You can also attach a directive to a Blanket, if you'd like to include every net within a specific area of a schematic.)Design > Update the PCB. The Class will be created and it will include each net you added in the schematic.Over to the PCB!----------------Design rules can be setup and used in many ways, so I'm going to show you an example of usage that I've been teaching students for the past few years. Others may have different approaches that are perhaps a little simpler, but I show this method because it highlights the various features built in and shows the way they can be used:Create a Width Rule-------------------In the PCB menu (Design > Rules) open the Design Rules dialog and create a new Width rule. Notice the new rule is named Width_1 and is set to Priority 1. This rule will be acted on first because it has the highest priority, so you can scope it to your new Class, then the other more general rules will be applied afterwards.Rename the rule to something sensible like Width_Power (or whatever your Class is called).Set "Where The Object Matches" to Net Class and choose Power from the list.Set different widths for Min Width, Preferred Size and Max Width, i.e. the common sizes you're likely to use on the board.(Repeat for Clearance rules)Switch Sizes on the Fly-----------------------When interactively routing (i.e. in Altium Designer press PT to route a track), while the track is being placed you can press several shortcut keys to affect the track with and other actions. To see a list of them, press the ~ button (above TAB) while placing the track.Design Rules can be setup to have a different track width for Minimum, Preferred, or Maximum. If you take the time to setup the rules properly then you can save a lot of time when routing by changing the width "source" during routing, to toggle between the three sizes you defined for Minimum, Preferred, or Maximum. The shortcut key for this is 3.Watch the Status Bar at the bottom of the screen, which will cycle from Rule Minimum; Rule Preferred; Rule Maximum; User Choice when pressing the 3 key.When you're routing you sometimes want to just type in a width. In this case, this time press the Tab key and type in a number and that will be the width. The track width will no longer follow the rules described above, but will specify the width source as "User Choice".The next time you route, the source will be remembered, either User Choice, Minimum, Preferred, or Maximum.One more subtlety: If you start routing from a net that is already partially routed, e.g. create a T intersection with another track, the width of the new piece of track will conform to the existing track if the source is set to User Choice at the time. Otherwise it will be whatever source you see on the status bar.Pressing Shift + W while routing will let you choose from a list of sizes, similar to pressing the Tab key and typing a size.Vias----While routing, if you change layer, a via is automatically inserted. The same technique can be used, see below.Pressing Tab while placing a Via from the menu only changes it for that instance. During interactive routing if you change layers such as by pressing * key or Shift+Ctrl+Mouse wheel then the automatically inserted via can be controlled by pressing Tab to specify a User Choice. This is also restrained by the RoutingVias design rule. Further control can be gained by specifying minimum, preferred and maximum sizes and using the 4 shortcut while the new via is inserted (watch the Status Bar cycle from Rule Minimum; Rule Preferred; Rule Maximum; User Choice). Pressing Tab will reset the setting to User Choice.Also when interactive routing and inserting a via, pressing Shift + V will choose from the list of favorite via sizes (defined in Preferences > PCB Editor > Interactive Routing).Best regards,James HarrimanAltium

author: technotronix
author_rank: Regular Contributor
timestamp: February 24, 2017, 11:16:52 am
content: Nice Solution provided by the Ice-Tea and ajb. I am using Altium designer from past few months and use to learn many things from Altium tutorial videos. Try to learn from videos. You may like it.