Resistor symbol value moves when rotated? - Page 1
Forum section: electronics / general

author: ryanmills
author_rank: Unknown
timestamp: February 28, 2022, 10:46:53 pm
content: I'm just getting into Altium after dropping Eagle. Most things I have figure out but I'm finding the default actions with resistors really annoying. Not sure if its a library thing or the default behavior.First resistor values don't show by default in schematics? Do you typically favor showing the part model number instead of the value? For me in the schematic I prefer the name and value only. Bit annoying to change it one by one.Second, I'm not sure if this is just TE packages but when I first place a resistor, the values are in random places, two different TE packages below. When I first place them the values are in kind of stupid spots, but when I rotate them magically they go to a good position. Examples below. So right now I have to enable the value then rotate each package before I connect it. Is this normal? Are there better libraries for common passives?

author: jwet
author_rank: Frequent Contributor
timestamp: March 01, 2022, 04:22:09 pm
content: Its probably has to do with the grid that the library part was created on. When you rotate it, it snaps to your sheet grid. You can test this but making a part.You can bulk change all the visibility of values, etc with the query tools. Its not easy to explain but its easy to do, look a the docs.Whenever I'm learning a new piece of software and it does bone headed things, I try to assume that the authors were smarter than that and I just don't know how to do it in the app. Usually its there, it just might not be used to what you're used to.

author: free_electron
author_rank: Super Contributor
timestamp: March 01, 2022, 06:14:43 pm
content: it depends how the library was created.if the parameters are not explicitly placed as a system string in the symbol then Altium shows only the value field by default and autopositions it under the designator.if the parameter strings are placed then altium will visualize them (provided they are not empty) in the order given. it will still autoposition.if the parameter strings are placed and LOCKED then autoposition does not happen.take a look at the fields indicated by the yellow arrows. There are a LOT of options... too much to explain. read the documentation

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 02, 2022, 04:18:05 am
content: Note that autoposition isn't grid locked; sometimes it is, but it seems more coincidence than intentional.I'm of the habit of tapping G a few times (to get '5' or 50 mil grid), select the offending labels, CTRL+SHIFT+D (or press A, G), then nudge them around (CTRL+arrows, or CTRL+drag then release CTRL), and finally set horizontal center alignment if applicable.This is a PITA so I tend to keep a row of symbols, so prepared, on the side of the sheet, as I'm composing a new sheet. Or paste from another sheet that's already got them handy. Just SHIFT+drag, or select and CTRL+R or CTRL+D, or select and CTRL+C, CTRL+V, to make duplicates. (Note that this works when using generalized components: you have an e.g. resistor, and intend to set the footprint, supplier link, etc. on the schematic; as opposed to having a library item for each and every part you would ever want to use and never editing their properties on schematic.)These shortcuts are, well some of them are fairly obvious, everyone has copy/paste; but Duplicate and Rubber Stamp are on the Edit menu, and SHIFT+drag you'll have to read the help I think, or discover it on accident.Note that Altium has some quirks that never went away from the earliest versions. Which, so does EAGLE, though I haven't used it, I forget what they are. One of the traditions is using sequences of letters as shortcuts; almost every letter has an associated popup menu. These are visible either on parent menus (including top level menus, which you can access in the Windows-traditional ALT+letter manner, or as a popup with the same letter, except for S), or Help/Popups.Likewise, options, lists, searches, etc. use Panels. Suggest keeping some sidebars open. See the above screenshot, nice thing about wide HD screens (much as they annoy me otherwise), you've got plenty of space either side to put the bigger toolbars like these. You can also snap them out as floating windows, which can be placed on secondary monitors if you like. (Remember to save these configurations from time to time, View/Desktop Layouts.) Minor bug: SCH/PCB List tends to lag a lot while it's populated, which is every time you finish an action (e.g. mouse drag). I forget if this has been fixed in recent versions. If you find this happening, try closing the panel, or switching it to only view selected items.Commands can also be customized by double-clicking blank space on the toolbar, or the DXP/(user icon) menu, Customize. This is quite advanced stuff, I suggest familiarizing yourself with the commands and default combos first, but just so you know where to find it when you're ready.Also remember to set autosaves (you can also change the location, default is some random gibberish AppData subfolder), and save your own settings (Tools/Preferences) once in a while so you don't lose any (many?) settings when it inevitably crashes. (It's wise to restart Altium about daily. There's enough memory leaks and rare funky behavior that it can get confused and start crashing after doing a lot of work.)Also familiarize yourself with the query system; this is still a rather cryptic function, and is certainly an advanced topic, so, get used to general workflow first -- but once you're ready for more, what you can do with it is select just about any combination of objects in the project, in one command. The one thing you can't do is relational queries (e.g. give me all objects that also match properties of another object); you can only query direct properties of an object. (Object Parameters are themselves an object, so can be queried by themselves, but also are a bit of an exception as they also show up under the object itself e.g. the HasQuery() function.) It did get significantly easier to use once they put in autocomplete, and query builder and helper dialogs -- give these a browse -- and you can also build a query with Find Similar Objects.Which, on that note, queries are how PCB rules work -- they added some basic built-ins for the most common cases: like for clearance, you get a matrix of applicable object types, and often this is specific enough for simple designs. It didn't always used to be this way, like back in, AD14 or something and earlier, it was just a straight query box (with the few preset examples on the drop list). So that's handy, but also you won't have to go very deep before needing to customize these rules. Something to look forward to, right?...Tim