pins and wires sometimes not connecting.
Why?
Youāve been playing with the Grid. Try to avoid that.
Youāll probably need to edit the library symbol to get it corrected.
Everything should be on a 0.05"/1.27 mm grid. ā corrected, sorry
1 Like
Thank you
My grid was: 0.5mil, 1.270 mm ā¦:
0.5 mil is doubtful. 1.27 mm is fine.
But something went wrong when creating/editing the symbol. I can see the ends not meeting correctly.
About the why partā¦
KiCad does not maintain a netlist internally at all (at the moment) and for connections it is solely dependent on attachment points of pins having matching coordinates with endpoints of wires. And as you already noticed, when the connection is recognized, the small circles and squares disappear.
In order for this coordinate matching to work properly, you have to work on a relatively coarse grid, and you also have to design your schematic symbols on a coarse grid. A grid of ā50milā seems to work best in the schematic editor (The PCB editor has no such limitation, you can use any grid you like on the PCB).
Some tricks:
If you have off-grid parts on your schematic, then select a big part (or the whole) schematic, then click the right mouse button and select Align elements to Grid from the popup menu.
Sometimes you want to place texts such as the RefDes or values off-grid, you can do that by first starting to drag them (which increments over grid dots) and then keeping the [Ctrl] key depressed, which disables grid snapping as long as you depress the key.
I believe the OP saying he/sheās using a 0.05"1.27 mm grid.
But that means the symbol in the library is āillā. Not knowing which it is, Iāve no chance of verifying it myself.
Me neither, but wolfgam can.
- Hover the mouse of the schematic symbol.
- press [Ctrl + e] to load it in the Symbol Editor.
- Check if the grid in the symbol editor is set to mills. (and set it to mills if itās not).
- Symbol Editor / Edit / Pin Table
Ideally all X and Y coordinates of all pins are on a 100mill grid, and thus have nice round numbers ending in two zerosā.
Two corrections:
You need to select the symbol, Hovering aināt enough. <_ incorrect, sorry.
Practically all symbols are on a 50 mil grid and should have a nice round number as paulvdh says. If you see a pin with a position like 251 mils, youāve found the culprit.
Are you sure?
For me it is. Just checked and verified it, but there may be some setting in the preferences which prevents this.
The KLC is 100mils. It is quite unfortunate that a bunch of the most standard symbols such as resistors and capacitors do have the connection points of their pins with a multiple of 100mil, but their center is on an intermediate 50mil grid. Fixing this would damage all older schematics when the library symbols are updated. Apart from a handful of symbols all will be on a 100mil grid.
However, because resistors and capacitors are so ubiquitous, working on a 100mil grid in the schematic editor is difficult, and using a 50mil grid tends to work better.
@paulvdh, I understand from another thread that you are now using KiCAD more intensively as a designer. I welcome that, connection to the real world is the best that can happen.
Concerning āhoveringā: yes, Iām certain. My installation is pretty default, and this is one thing I never bothered to modify (I never even used the ctrl+e shortcut before reading your post).
KLC is one thing, reality is another. I randomly selected the most ubiquitous gate in the world, the 74HC00, and itās outline is on a 50 mil grid. The same goes for all other 74xx gates and a mountain of other parts, thus my reason for using a 50 mil grid.
The pin ends are correct on 100 mil, though.
Also note I did write **ideally** when I mentioned the 100mill grid.
In practice you could also set the grid to as small as 25mil, but that is about the smallest to be practical for connecting wires.
Well, me to, KiCad does inherit some settings from previous installations (at least I think so), but hovering and activating a hotkey on the hover location has been standard from at least KiCad V4, or, for as long as I can remember.
The whole TTL / cmos libraries are probably from before the KLC existed.
KLC is a reality too, but itās not perfect, just like the rest of reality, but I still like itās intentions and try to follow them.
50 mil has been a good compromise for me as schematic grid. YMMV.
I use 50 mil and stick to it ! also with my new install of 7.07 if I hover over a symbol and press āeā I go to symbol properties and if I press āctrl eā it gets loaded to symbol editor. I do not have to select the symbol and I installed the latest stable release about an hour ago so this is ādefaultā if that helps.
It does. I just closed down KiCAD and tried again and now it works.
1 Like
Smells like yet another small usability bug. Iām also not sure that closing KiCad made the difference. I discovered for example that when the āauto wireā function is activated when the mouse cursor is near a pin, then the hotkeys are disabled. (I have not reported that one yet).
Is there a plan to change this? One of the things I dislike about KiCad is that nets are not stored as objects, but rather are dependent on overlapping wire endpoints. I would encourage a change to an object-based storage scheme. (Not that anyoneās asked me!)
As this is off-topic, replies should probably be in PM or the discussion forked into a new topic.
The pin / grid discussion is pretty much answered and exhausted, and I do see it as (somewhat) related.
If it continues too far off topic, I (or another person with Super Powers) will split it off into a separate topic.
Just a few days ago I made a feature request on gitlab for ratsnest lines, and now I realize a real netlist in the schematic is the underlying, and wider issue, so I changed the title.
It started in the user forum topic below:
And a link to the gitlab issue. You can give this gitlab feature an upvote, and/or add a comment for other use cases where having a netlist in the Schematic Editor is an improvement.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.