I am new and trying to create a very simple, but odd-ball PCB. It is a 0.90" round board with a large pad on one side to serve as a coin cell + contact and a solder pad on the back for a soldered wire connection. A single via to connect the two sides and probably a short trace on the back.
I created two new footprints, one for each side of the board. When I created them I wanted to be able to easily establish the proper geometric relationship between them on the PCB so I first drew an outline circle and a short line on the User 1 layer. I then drew the front side copper pad using two rectangles with round corners placed at the same center but at 90 degrees so they overlap and form a + sign. I figure that is a good way to show the polarity for the coin cell, a point that many battery holders do not implement well. So my first question is, will two pads superimposed on each other work OK?
I then copied that footprint and altered it for the rear side pad. I kept the circle and line on the User 1 layer. And saved it with a new name. Now I am creating the PCB and have used the two footprints. The outer circle allows immediate positioning which is guaranteed to be correct. but now there are two footprints with the circle and line on the User 1 layer. Is this a problem? Does it even get included in the Gerber files?
Final question, and perhaps I have not watched enough videos or read enough, but how do I know that my correct board outline is established? I have placed a 0.9" circle on the Edge Cuts layer. Is that it? Is there any chance of the 0.8" circles on the User 1 layer could be misinterpreted as edge cuts? I wouldnât want that. Can I delete them in the PCB Layout without causing a problem with the footprints?
Two pads over each other are OK. When they have the same pad number, KiCad will treat them as a single pad. If they do not overlap, then KiCad will draw a ratsnest line between them in the PCB editor until you connect them. This is used quite extensively in KiCadâs own libraries too.
I guess you want to connect the big âplusâ to the battery, but you will have trouble with the solder mask. It may or may not overlap the pads a bit and possibly interfere with the electrical contact.
I tinkered a bit with your project.
Exported both footprints to a library.
Added a schematic, project file (You should never create a PCB without a project, KiCad does weird things without a project (Itâs called âstandalone modeâ).
renumbered pads: Tab: Clearance and Overrides set the Solder mask expansion to 0.5mm this is probably enough to ensure the soldermask never overlaps the pads.
On the Plus footprint, for the pads:
Made the references (J1 and J2) invisible on the PCB.
Something happened to a circle, but Iâm not sure what ???
PCB Editor / Inspect / Design Rule Checker is now error free
For your other questions.
Gerber files are one layer per file (you can zip a whole set), and you can control which files you generate, and which you send to the Fab. Also, do not forget to generate drill files and include them too, or there will not be a vial. Only graphics on the Edge.Cuts layer is part of the PCB outline. You can add internal routing too.
You can also examine your Gerber files in KiCadâs gerber viewer, or upload them to an external viewer. Several PCB manufacturers have a viewer you can use to preview your design before going though with the ordering. Ucamco also has an online gerber viewer.
I started with the small pad to the top left,
Placed it in the centre of the cross hairs
Drew the cross using the âDraw a Graphic Polygonâ feature.
Right mouse click on the centre of the cross and pad then selected âEdit pad as Graphic Shapesâ then âFinish Pad Editâ
Now I have a single pad shaped as a cross.
Paul has covered the rest except: Are you happy with only one via?
Maybe have a couple of spares attached?
When new KiCad main number (7) version is changed there are lot of bugs that are fixed later.
I skipped 7.0.1 and probably 7.0.2 starting from 7.0.3.
Last number change means only âbug fixesâ no other changes.
Now there is 7.0.9 that certainly has much, much less bugs than 7.0.2.
Given you want a PCB diameter of 0.9inch (22.86mm) I will assume the PCB/Battery slip into a pocket in some housing.
Further, you indicate wanting a âCrossâ for the +contact surface.
Given that is correct, I suggest you Not use a Cross for the +contact and these comments may be worth consideration:
⢠A battery sitting on a PCB contact surface offers zero physical loading such as to apply pressure/loading to ensure good contact. Even if a Spring above the battery presses it down - You will have reduced surface-area for contact (compared to a fully filled diametrical circle, especially one having raised metal/leaf-spring as you may find in commercial products wherein they have formed-spring-beams/etc). Iâd wager a cup of coffee that you canât find one with only a Flat-PadâŚ
Temperature may cause expansion/contraction and only a tiny amount is sufficient to cause problems.
Well, come on by and I will have your cup of coffee, your choice of flavors. I have a well stocked coffee cabinet. Tea too, if you wish. Even hot cocoa with mini marshmallows.
So, your point is well taken. Yes, I do have a pocket in a solid metal device. And a plastic insulator that holds this PCB. I have in mind a screw-on cover but that part is not designed at the present time so some flexibility exists.
I donât suppose that you have a source of the spring contacts that you mention. I would gladly buy some at a decent price, but my project is for a device that must be made with minimum cost. An additional part, the spring contact, that must be fabricated would add significant cost or effort. But I will make a search.
Perhaps a standard spring can be added to that screw in cover.
As for the solder mask interfering with the contact, I see no reason for a solder mask on this side of the PCB. Nothing will be soldered to it. I am also concerned about the thickness of a silkscreen because I would like to also have some legends on this side where they would be visible. I know of no way of finding out about the relative thicknesses of a silkscreen and copper layer other than to order some PCBs and check them. I suspect that this may vary from one fabrication house to another.
And there is one more consideration. I donât know about you, but I have personally observed an enormous number of battery holders that have used spring contacts made of an alloy that is not resistant to corrosion. And I have had to repair those spring contacts when either battery leakage or other, perhaps external substances have caused corrosion. Those alloys were chosen for ease of soldering, not corrosion resistance. So, perhaps a standard stainless steel spring could be used attached to the screw in cover.
Re: jmkâs Graphic Polygon method for making my big cross contact.
I was tempted to use the Graphic Polygon but was not sure how to have that polygon filled with a copper pour. Are you saying it will be filled automatically, with no further actions on my part. And any pad inside that area will be incorporated. So it all becomes that pad.
I am going to start over and try it this way.
And why would I need to have more than one via or plated hole to transfer the net to the other side? My current will only be around 2 mA. Is there a problem that I am not aware of?
The three drawing tool with internal shading have the ability to be filled. Fillets can also be altered to change corners.
Double left mouse click or hotkey E to enter properties and experiment. Right mouse click to enter selection.
The line drawing tool will not fill, use polygon tool.
Depending on if the âfillâ box is ticked when using the function.
Yes.
After creating a shape place a pad (any size) inside. Right click pad and select âEdit Pad as Graphic Shapeâ or hotkey Ctrl + E. Use Ctrl + E a second time and the whole shape becomes the pad.
Just an inherent mistrust of using single vias wherever any power flows. Signals, OK, power, nup.
Iâm not sure of the result of some idiot shorting out the button battery in situ and I donât know the current capabilities of said battery, but anyway, JMHO
I uploaded my mods as a complete zipped project. See above.
Nearly every PCB manufacturer will apply a solder mask. Solder mask is also a ânegativeâ layer, you specifiy where the mask has to be removed. If you do not include a solder mask layer with your project, then it is quite possible your whole PCB will be covered with solder mask. So be careful here.
Yes. changes in the third number of KiCadâs version numbers are bug fix updates. There are no new functions added, nor a file format change. These bug fix releases are released around once a month and they have around 70 bug fixes each month. Less bugs is a good thing, and compatibility is excellent. On my Linux box, KiCad updates are pretty much automatic, because updating programs is a function of the OS itself. I just tell my Linux box to update all software once every few weeks, and then it does that for me. (It is possible to automate that, but I do not like automatic updates).
There is only one gotcha. Sometimes the KiCad developers overlook something silly, and a âbug fixâ update introduces a mayor bug, which may even make KiCad unusable. If that happens (and it happened a bit too often), Then the KiCad version gets replaced by the next bug fix update very quickly (usually within 2 days). If you do not want to risk this, then wait approximately a week after a KiCad update before you install it.
That worked. Using âEdit Pad as Graphic Shapeâ or hotkey Ctrl + E twice is certainly not intuitive. I never wold have guessed to use that. But it did work.
Thanks! Now if only I can remember that trick for the next time I need it.
Great. I am trying to do it again myself first so I can learn. Then I will look at your project and see how well I did. Yes I need to do this project, but I need to learn KiCAD more.
I appreciate your comment about the solder mask. It sounds like I need to include that layer with a mask that is larger then the board if I want none at all. Or at least keep it well clear of the copper.
And I went ahead and did the upgrade. It seems to have gone well. My work, including the custom footprints and symbols is all there - I was worried about that. And everything seems to be working as before.
Thanks to all who responded for everything! It has been extremely helpful.
As the cover is not yet designed and youâre concerned about battery leakage/acid-corrosion, consider Spring-Loaded-Pogo-Pins for contact but, designing the gizmo will need considrations⌠and we (I) know nothing about the physical envelope that will contain it so, itâs difficult to comment.
Iâve seen many, too many batteries leak but, at the moment, I donât remember any Coin battâs leaking though, Iâm sure they do. I have one sitting here that is swollen so, it may start leaking but, itâs been like this for two years and still provides enough power⌠look at the swollen profileâŚ
