Is it possible to keep a string appended to a parameter text? - Page 1
Forum section: electronics / general

author: hkBattousai
author_rank: Regular Contributor
timestamp: July 10, 2014, 04:04:25 pm
content: When entering value for and inductor or a capacitor, it is easy to write "5nF" or "2mH". But in the case of resistors, it is not easy to write "1?" every time since ? is not an easily typeable character.Is it possible to keep ? always there, and make it hidden when editing the label. Same thing is done with multi-part components. There are capital letters A, B, C, D, ... appended to them, and they disappear during editing, then they reappear as soon as the editing finishes.Can the same thing be done in general; especially for resistor value labels?(EDIT: The Greek character "Omega" is replaced by question marks (?) by the forum software. All of the question marks in mid-text are actually the Omega character.)

author: Araho
author_rank: Regular Contributor
timestamp: July 14, 2014, 10:24:16 am
content: The omega character isn't really used in schematic labels as far as I know. Every project I've seen use R or K/M/G instead of ? (omega) to say that this is a resistance. If you have a resistor greater than 1kOhm, like 1700 ohms, you write just the k: 1k7. If you have a resistor smaller than 1kOhm, like 800 ohms, you use R: 800R. R can also be used to substitute the decimal point, for instance in a 1.7 ohm shunt resistor: 1R7.The reason this is used, as far as I've learned, is that decimal points are hard to see on a printed schematic and the omega symbol doesn't always show up on every computer etc. This makes it easier to avoid reading errors.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 14, 2014, 02:24:07 pm
content: For that matter...Has anyone else done this before?Print a PDF of your board, with a diameter dimension somewhere on the PDF, using the "slash O" symbol to indicate diameter.Every time I've seen it, it produces ":" in the output. Sigh...Regarding component values, I just as well leave the suffix off; it's not required. That's partly what the symbol is there to indicate. Traditionally, simulations don't use the suffix (it's stripped off anyway).Personally, I've always labeled resistors with no suffix whatsoever. This is normal for average values ("10k"), but looks kind of odd around small values ("1"?). One tip is to write the full value given the precision: a 5% 1 ohm resistor should be "1.0", which gives you some idea that it's actually a label for the component, not just... a random digit floating around the schematic, or an accidental pin number, or something.Another, not really pet peeve, but a gotcha that not everyone is very clear about: multiplier suffixes m, u, n. In the US, capacitors are almost exclusively written in F (supercaps), uF or pF. (Often, one or the other is dropped conditionally, as defined in a note somewhere: for example, an electrolytic might be "10" (10uF), and a non-polar might be "150" (150pF).) It's more common these days to see 1nF instead of "0.001uF" or "1000pF". It's still quite uncommon to see "10mF" instead of "10,000uF" though (a caution due to the days of MFD = "microfarad").Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 14, 2014, 02:33:01 pm
content: Oh, and as for actually DOING it,No, I don't think there's a way to do that. Edit the string manually, inserting text and not deleting the Omega. Put the character in your clipboard so you can replace it easily.You could also do it as a finishing step: go to SCH Filter, select All Objects, 'Open Documents of the Same Project', Objects passing the filter = Select, Objects not passing = Deselect + Mask out, criteria "IsComment" (or whatever your labels are -- another example would be, "IsParameter AND (Name = 'Value')", etc.), Then in the Inspector, include all objects from open documents of same project, go down to the "Text" field and hit the "..." button. Formula tab, enter "! + 'Omega'" (that is, paste in the Omega character), hit OK....Uhm, crap. In AD14.2 I'm not seeing a "..." button for the Text field. Thanks a lot Altium. And nevermind.Tim

author: free_electron
author_rank: Super Contributor
timestamp: July 15, 2014, 06:10:28 am
content: Quote from: T3sl4co1l on July 14, 2014, 02:33:01 pmwhich is normal behavior as that is NOT the way to do it ! The comment field is a PARAMETER which is driven from the library or vault.Once a part is placed you do not edit the value. you can toggle it from the library value to other parameters (for example set it to =Supplier1you can add parameters on the fly: in the schematic inspector open the tab 'parameters' and click 'add user parameter'. there create something called 'value' and set that to whatever you want.The part comment (which we use typically to show the value) is NOT binding. it is only a comment.it is WRONG to manually edit this in the schematic.The component designator IS binding and you can alter it through a formula. (select two capacitors and you can enter an expression to alter it.Parameters can be driven from databases.

author: free_electron
author_rank: Super Contributor
timestamp: July 15, 2014, 06:18:01 am
content: back to the original postNEVER use greek characters like omega and mu. and NEVER use comma's or dots in part values.1 ohm is written as 1R0.1 ohm is written as 0R11K is written as 1K1 microfarad is written as 1uF2.2 microfarad is written as 2u2optional :1 ohm 1% is written as 1R01 ohm 0.1 % is written as 1R00but : precision resistors typically have a different symbol or no special markings. this stuff is pulled in the BOM. do NOT overload the schematic with text. Schematics need to be clean.A diagonal line over a corner for example (see image below)dots tend disappear in copies or scaled prints.font sets are not necessarily translatable. not all font sets contain the greek characters. so avoid those.

author: tautech
author_rank: Super Contributor
timestamp: July 15, 2014, 07:48:46 am
content: Confusion reigns supreme if accepted convention is not used in schematics.The problem is that conventions differ and standards are not universal.There are many subtle differences in schematic components, the different core types used in inductors for example.Back to topic, the OP and free_electron have for resistors used the rectangular box that is accepted in this part of the world, and because everybody knows this symbol is a resistor, whats more it is marked with an R, there is just no need to signify Ohms, just make it clear where the decimal point is exactly as free_electron has.One that annoys me is the 2 conventions widely used for logic gates.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 16, 2014, 12:26:36 am
content: Quote from: free_electron on July 15, 2014, 06:10:28 amSo by your instruction, I should have one single-use library part for each e.g.TP1 +VTP2 +5VTP3 SDITP4 SDOTP5 VINTP6 ISENSETP7 ..Fuck this, you get the idea. I can literally go on for two hundred plus. Because that's the case for a small design. You're kidding yourself.And I'm supposed to manage all the footprints at the same time? And supplier links? And symbols if they should ever change?!Tim

author: Laertes
author_rank: Regular Contributor
timestamp: July 19, 2014, 07:45:30 pm
content: Quote from: T3sl4co1l on July 16, 2014, 12:26:36 amWell, TPs are a rather special case in which the comment is completely valid to be changed. However, you don't put the value of a resistor into the comment and you sure don't change it after placement... you have a 1k 5% 1/10W 0603 Resistor library component and you have one for 3.3k 5% 1/10W 0603 etc. That's the way it's supposed to be done in Altium, as for example the way AutoBOM works in AD13/14 clearly shows.And maintaining that is quite easy if you do use a DBLib or the Vault.My company decided that vaults suck(though I'm not sure why), but we do have migrated all the individual intlibs each designer kept around and used for his projects to a single, company wide(that is, the five people actually working with AD) database library and now I cannot imagine how we lived before it. All the stuff just always works, like for example updating from library after some part of the component has changed never screws any parameters you manually changed up anymore, AutoBOM always has all parameters correct immediately etc. Also, managing the library itself(adding components, adding footprints etc) just has a very nice workflow now. And everybodys schematics automatically follow the same conventions regarding the parameters, too.If you do work alone, just set up a database library to use an excel sheet as the "database" and you're good to go. If there's a group, maybe it's worth the time to setup a real database and put all your libs on an SVN server...