is there are improved way of doing this in Kicad 6.x?
I applaud you for reading though the forum and finding and reading about a topic that is similar to a problem you’re struggling with. KiCad has changed a lot though in the 5 and a half years since this topic was created, and reading though all of such an old topic and making a summary of everything that has changed and may be applicable to your situation is too vague a task to start working on.
For this reason I expect this topic to be closed as soon as a moderator sees it’s been dragged up.
If you are stuggling with a similar topic, I suggest you start a new thread with a description of your own problem (and possibly also link to this old topic).
1 Like
Excellent suggestion. The software now closes topics after 3 months of inactivity. That works out quite well in this forum because sometimes the method has changed dramatically since the implementation.
In KiCad V6.x there are many snap points used while creating dimensions. Including the center points of arc’s, circles an holes.
I find it even impossible to turn the snap points of holes off in KiCad V6.
Even if I turn off everything in the selection filter it still sees the holes as snap points:
And if I then turn off all magnetic snap points in: PCB Editor / Preferences /Preferences / PCB Editor / Editing Options / Magnetic Points (For pads, tracks & graphics) then KiCad still uses the holes as snap points.
You can recognize that KiCad sees a snap point because it draws a small circle around it.
1 Like
FYI -v6.0.4
No problem snapping to center of hole.
If I hold the Command-key down (on Mac), then No Snapping.
hummm, that’s not what i mean…
The issue is the wire/via tools won’t snap in the center between two pad/via/holes, even i draw a wire in between, it won’t snap to the center of the wire.
first thing first, please ignore grid, we are only talking about snapping to other things.
what im trying to do is draw a via in the mid of two pads. (the via in this pic still not perfect center)
I tried draw wires/lines between pads to determine where is the perfect center between two pads.
then as you can see, the via tool won’t snap to intersection.
see my gif on next post since im not allowed put two embedded element in one post
here is the video
There is a combination of things happening here.
First, there is no snap to midpoint in KiCad. KiCad is not a mechanical CAD program, but a Schematics and PCB design program.
The quickest way to do what you want is to first define a custom grid with half the distance of your GND pads. For more complex graphical things in KiCad, it is usually better to first design it in a mechanical CAD program, then export as .DXF and import that in KiCad.
But more important, I’m guessing you are trying to make something that you should not be making in KiCad. What is the goal of the array of GND pads and the via’s? If you tell us the broader picture, then we can probably give much better advice.
1 Like
First, there is no snap to midpoint in KiCad. KiCad is not a mechanical CAD program, but a Schematics and PCB design program.
I’m not looking to achieve this directly by Kicad allows me snapping the mid point of a line, it’s nice to have though. I can draw lines that helps me find the mid point, then the tools should allow me snap at the intersection at least.
Also, I do not consider place a via in mid of two pads is unreasonable for a PCB designing tool, sure it won’t be full fancy CAD replacement, but it should have basic features like this.
The quickest way to do what you want is to first define a custom grid with half the distance of your GND pads. For more complex graphical things in KiCad, it is usually better to first design it in a mechanical CAD program, then export as .DXF and import that in KiCad.
It is really hard to match the exact point in this way. A better workaround would be using drawing tool draw lines as shown in my gif, then place the gird origin on the intersection, since “place grid origin” is able to snap.
My point is, the drawing tools already have the needed function, it won’t be hard to provide the same thing on via tool and wire tool.
But more important, I’m guessing you are trying to make something that you should not be making in KiCad. What is the goal of the array of GND pads and the via’s? If you tell us the broader picture, then we can probably give much better advice.
What I’m trying to do is avoiding put through wholes on ground pads, since in that way when manufacturing those wholes will suck solder away, weakening the joint.
then your vias will naturally snap to the exact midpoint between the pads
1 Like
This doesn’t answer your question directly, but have you consider making an array (right click on via → special tools → create array ) of those vias? As I see it you seem to have a regular spacing, it may be easy than drawing help lines, place via and then delete help lines.
I gave it a try on my KiCad v6.0.5 and the via snaps nicely to my track, if I draw tracks as guides, if I make an “X” as you shown in your gif, it “tends” to snap to the middle point if you are careful, using the full screen cursor, helps you to confirm visually.
This is only a small part of what you are trying to do.
To me it looks like you are trying to design a footprint in the PCB editor.
There are many examples of footprints with thermal pads and via’s in Kicad’s default libraries.
To examine what they look like, just start the Footprint Editor and do a search for the word “thermal”.
About the grid…
thebigg already repeated that it should be easy this way. I think the step you missed is to first define a custom grid, which has the right distance (of half the GND pad pitch). You can set a custom grid in PCB Editor / View / Grid Properties
In normal situations it is indeed good to avoid putting via’s through SMT pads, but these big thermal pads are a bit different. Because of their big surface area they will not be starved of solder. Having the via’s suck up a part of the solder can even be beneficial. Too much solder on a thermal pad forms a cushion on which your part floats, and this prevents good soldering of the “real” pads, and via’s filled with solder conduct the heat better.
Via’s normally do snap to tracks. There are some settings for this in PCB Editor / Preferences /Preferences / PCB Editor / Editiong Options / Magnetic Points
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.