OK, going to prefix this with an apology, totally new to KiCad and also using a plugin to pull the board info in from inscape, so expect that’s going to complicate matters?
So I have a hole that is meant to be 3mm, but in KiCad it’s closer to 3.4mm (not a huge issue, but would like to work out a way of fixing it before it eventually does become an issue!)
Thank you for your time!
First:
Why do yo post images on imgur and then link them from here? You can just drag an image from your file browser into the text window of your post and drop it here.
About those holes…
I do not know what those grey circles are, but they do not look like holes to me.
One way to do it in KiCad is to place via’s, and use them.
The size of a via can be changed by hovering over it, then press e for edit, which opens it’s properties window:
There are some draw backs to using via’s.
The most obvious is that Via’s are very volatile in KiCad. Via’s that are only connected on one side can even be removed (accidentally) by DRC. Via’s also easily get pushed aside by the Push and Shove router, so you have to disable that too. Via’s also do not have pin numbers.
A more subtle drawback is during Gerber file creation. If you accidentally “tent” your via’s, they get covered by solder mask, and you can’t solder wires to them.
So overall via’s are not such a good solution.
Replacing your holes with single pin footprints (For example “Test Pins” is a more robust solution. Use: ** Pcbnew / Place / Footprint [o]**. Then type in “test tht” (with a space, so the RegEx. search searches for both sub-strings, and then select a footprint that looks nice from the list:
After you’ve placed a testpoint you can select it, press e for edit and change it’s properties. Be careful what you select. If you select the footprint, then you edit the footprint properties. If you select the (single) pad in the footprint, then you edit the pad properties, and can change annular ring size or drill diameter, and much more. A pad has many properties, so a big window to set them all:
By using real Footprints you ensure that you can generate valid Gerber files and have a PCB manufactured.
First:
Why do yo post images on imgur and then link them from here? You can just drag an image from your file browser into the text window of your post and drop it here.
Sorry, I didn’t know that was an option. Tend to use Reedit over forums where imgur is the done thing…I will stop doing that here!
About those holes…
I do not know what those grey circles are, but they do not look like holes to me.
KiCad seems to see them as holes, at least in the 3D viewer, have not generated any Gerbers to check…I should probably check that, but one problem at a time!
Edit to add:
This is what I get when I hover over the grey thing/hole? and press E
Your workflow is different from the usual workflow in KiCad, and that can be the reason of your holes looking differently. Maybe they’re covered by solder paste, or any of a dozen other things.
I often have a different way of operating, (which drives other people, especially “teachers” crazy sometimes).
I tend to “fool around”, experiment with features. “What is this?”, “How does that function work?”, “What are the caveats when I do it this or that way?”.
I can spend quite a lot of time on that, without making any visible progress. And then, when I’ve gotten familiar with a decent sub-set of the functions I can do a conversion relatively quickly.
Another way is to do it step for step, “One problem at a time!”, and this looks like steady progress. But you may well spend a lot of time of getting one of the intermediate steps right, and then discovering three steps later that you should not even have done that earlier step at all.
Therefore I recommend to fist get to know KiCad and how it works. Use your existing project, but just punch in some holes at random locations, and verify all the way to the Gerber files that these holes are defined as they should be.
For such tests you just need a few polygons and a handful of holes, which do not even need accurate placement. If you skip the “neat” steps, and the repetitive operations of getting 100 holes right, you can do a lot of experiments in a short time frame.
---- 8<------- 8<------- 8<------- 8<------- 8<—
And now the only remaining question is:
What does a handful of holes look like?
That’s a very polite way of putting it! 
Right now my workflow is Scan a PCB > import into Adobe Illistrator> Trace the Bord> Export as an SVG> Import into Inscape> Use a Plugin to export the SVG layers into KiCad> Export Gerber…
Of the top of my head, sure just adding the scan into KiCad and tracing with the base tools would be much faster and trouble-free…but there is a large part of me that wants to get this workflow to work, not for this PCB so much, but for projects in the parts and future that. And I just find the concept of Art to PCB interesting. But, I am very cognisant that I’m not making life easy for myself here!
I will heed this warning, as frankly you have been so helpful, and think you are right in this case.
Sooo…I exported the gerbers to see if the holes would even show up…And I think they did, just uploaded the files to a popular far east fab site (not sure if names are permitted here, got slapped on the writ in another forum for mentioning them by name).
So, now it a question of the size…do I find a way of reworking the current mystery pad styles I have, or can I replace them keeping their location (as it’s all for nothing if I lose the precise positioning) or Is there a way to adjust them in the drill file??? I think I will go and start watching youtube videos on KiCad basics and wait to hear back for someone far better suited to tell me what approach to take, as frankly I don’t know what I’m doing…you saw my workflow!
You do not need to use the web just to look at a gerber file.
KiCad has a bundled in Gerberviewer, called “Gerbview” 
and this is a decent Gerber viewer, and can also load drill data.
It is possible to modify drill data with a text editor, but it’s error prone, and “volatile”, as your edits will be overwritten if you generate the Gerber / drill files again. If you click on your hole, and then press e for edit you probably get a popup window, and can possibly change the drill diameter.
Also, when you place a footprint (of for example a test point) on your hole, there is a good chance that it recognizes your hole as a snap point, and coordinates will be the same. I made extensive use of this in:
KiCad-nightly V5.99 also already has a: Schematic Editor / Place / Add Image and this can load a background image in Eeschema, which can be useful for retracing a schematic.
Here a simple screenshot of an experiment. I imported a B/W picture of some random schematic, and placed a few KiCad schematic symbols over it:
Something similar for Pcbnew would indeed be very nice. Import some color images from a PCB (converting to BW looses too much info). Images from both front and (mirrored) back, Some even go as far as sanding to get to bare copper or even inner layers, so a “bunch” of pictures, and with transparency would be real nice.
If you like this, then go up vote:
Thank you!
No joy there, unless I need to change the grid in someway, seems to always want to snap to the nearest grid point, rather then the hole.
Couldn’t see a resize option looking at it…but not 100% what I’m even looking for…I guess a nice shiny button that says ‘DRILL SIZE’? I just get this:
And, on my long list of issues, I just noticed the plugin puts all Drill points on the layer that gives them a via annular ring, not sure if that is an issue if ordering single-sided PCBs, but still. another issue to add to the pile.
Made an account just to upvote, I’m going down the KiCad rabbit how that is something I want to see!
There is not much I can predict from a bunch of grey pixels in a circle
You get a popup for a footprint, so at least it’s some sort of footprint:
And it resides in this library:
Which is a non-standard library, so I don’t know what’s in it.
What you can do, is modify the library footprint with a decent pad and/or hole, and then update all footprints on the PCB, which gives them all the same hole.
Or, even simpler. Use the: Change Footprint button on that dialog, and then replace your hole with Test-point. (There is a selection under there, which asks you if you only want to change a single instance, or all similar footprints.)
And there are plenty many more tricks in KiCad.
You star, that worked a charm!
Guess the next stage is learn how to edit existing footprints like ‘Test-point’ and customise them to my needs…this is progress!
Simple answer, Hover over any existing footprint in Pcbnew, then press [Ctrl + e] to edit it in the “Footprint Editor”.
The Footprint editor Icon is in KiCad’s project manager, between Pcbnew and Gerbview.
If you do it this way, the modified footprint is directly put back on the PCB. If you want to change the library footprints, then you also have to do some:
(KiCad’s default libraries are read-only, so you have to make copies of footprints).
Perfect, now have a beautified 3mm hole no through plating in just the right place…I will sleep well tonight!!!
Thank you so much for all your help.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
