LTspice: How to display numeric voltage value at a specific node in schematic? - Page 1
Forum section: electronics / projects

author: Greybeard
author_rank: Frequent Contributor
timestamp: August 29, 2025, 08:50:18 pm
content: Hi,can anyone tell me how to display a numeric (DC voltage) value at a specific node in the schematic?I found the attached amplifier simulation somewhere:When loading the .asc-file, three ominous question marks appear in several places in the schematic.However, after the simulation run, the question marks were replaced to DC voltage values. Great!I tried editing or copying these three question marks to use them in my circuits, but it didn't work.I tried to google search the topic without success (probably because I did not use the correct search terms).Can someone please explain to me how I can insert these three question marks into my own circuits?

author: ledtester
author_rank: Super Contributor
timestamp: August 29, 2025, 09:23:52 pm
content: I think this is what you are asking about:https://electronics.stackexchange.com/a/535014/95488On the Mac version you can use the right click -> Draft -> .op Data Label menu item (see attached screenshot).Note that only the DC operating point is being calculated (i.e. the ".op" Spice directive). I doubt this works for a transient analysis.Update: It does work for transient analyses but only the DC operating point is shown.Update 2: The .asc file has these expressions for the data labels:Code:DATAFLAG 1680 -192 "round(10*$)/10"DATAFLAG 1648 464 "round(10*$)/10"DATAFLAG 1984 -112 "round(10*$)/10"DATAFLAG 1984 384 "round(10*$)/10"DATAFLAG 2336 -112 "round(10*$)/10"DATAFLAG 2304 368 "round(10*$)/10"DATAFLAG 1776 16 "round(10*$)/10"DATAFLAG 1776 240 "round(10*$)/10"These expressions format the value in question to a single decimal place.

author: Zero999
author_rank: Super Contributor
timestamp: August 29, 2025, 09:32:38 pm
content: That file contains a symbol which isn't part of the default part of the LTSpice install. Please post the .asy. The forum doesn't allow that extension so append .txt to the filename.

author: Greybeard
author_rank: Frequent Contributor
timestamp: August 29, 2025, 10:41:25 pm
content: Quote from: Zero999 on August 29, 2025, 09:32:38 pmIt's the transformer:

author: Greybeard
author_rank: Frequent Contributor
timestamp: August 29, 2025, 10:52:01 pm
content: Perfect explanation, Ledtester!Thanks!

author: Ian.M
author_rank: Super Contributor
timestamp: August 29, 2025, 11:13:58 pm
content: You can display *any* expression computed from the node voltages and currents of a .op analysis. Many of the other analyses implicitly run a .op analysis to determine their initial conditions. Seehttps://ltwiki.org/index.php?title=Undocumented_LTspice#Operating_Point_Data_Labels_.28visible_numeric_dc_bias_values.29They are unfortunately not useful if you use .tran startup as the operating point is calculated with all DC sources zeroed, and can be very confusing if .step is used. Also a major limitation is they *ONLY* display .op data, so cant be used to display the results of .measure statements.Incidentally the SPICE3 .print command used to select data for tabulated output, doesn't produce output under LTspice. Instead it aliases to .save which excludes all data not explicitly specified from the plottable results.