DB62 and Pin Receptacle Symbols

Schematic
62

Tracks can be locked with the l shortcut key.

Footprints can be locked via their “edit properties” window.

I do not know how to lock graphicse on Edge.Cuts, this seems to be missing in KiCad.

Grid origin can be adjusted via:
Pcbnew / View / Grid Settings
Or you can use the grid icon in the lower right side of Pcbnew:
image

63

Thank you @paulvdh. Good information.

How do I print off a paper version of my PCB so that I can lay my actual one over top and see how my holes line up? Is that possible?

64
65

My bad. You did put this in a post above. I thought I read it somewhere and couldn’t remember where. I have read so many things about KiCAD my head hurts. I will print off my PCB and see how it looks. Finger crossed. Then I have to clear up my ratsnest.

66

One? :sunglasses: Did I miss someting?

67

image

LOL @jos
Okay couple more questions.

  1. Where my 62 pin connector mounting holes are, I think I need to put a couple of mounting pads there as well, is that correct? How do I go about doing that without disturbing too much?
  2. Also, there are six mounting holes around the perimeter of the board. Do I go back and put them on the board as mounting holes and then as NPTH Mechanical? Can I do this on the PCB board only or do I have to start somewhere else?
68

  • Pads are not out of place if the space is available and potential electrical isolation requirements are being met. Just make sure there is enough clearance for the actual mounting elements like washer, nut, rivet, etc. M3 washers can take already about 7mm in diameter, and a nut pretty much the same. On top of that you might want to consider the bit to tighten that nut. Even a pop-rivet tool would need extra space.

  • There are a bunch of mounting holes pre-defined in the libraries as NPTH’s. Key for NPTH is to set drill size and pad size the same. Best practice turns out to be to place mounting hole symbols on a schematic in some out of the way place. Assign a suitable size NPTH footprint to it. F8 and you are set.

69

Thanks @jos. Good advice. I will see if I can get it right.
Not sure if you answered the first question about the 62 pin mounting pads? These are solder terminals as you can see from the image. There are two tangs that push through the hole and then solder to the backside. How do I put pads there without messing up my PCB layout?

70

You are right. Appologies.

As for the actual pads for D-sub connectors it’s always been somewhat of a challenge to keep a balance between anular ring and to get sufficient connection to the middle row. It’s a bit like BGA design.

You could play with different anular ring size top and bottom. That should work.

71

Sorry maybe I didn’t word it right? Remember this is somewhat new to me. So I am at the stage of building my PCB. What are the correct steps to go back and place these two pads for the D Sub and 6 holes for mounting without moving a single thing on my PCB? I have this thing dead on as I printed it out and compared it to my sample. I do not want to move anything if I don’t have to.

72

I don’t know if anyone else is confused, but I think you are talking about copper around the two mounting holes to provide somewhere to solder the mounting tabs of the connector. If I’m right then that should be part of the footprint. Looking at the screenshot you provided, above, of the board layout with all the ratsnests, it does look like there is probably an annular ring (pad) around those mounting holes. If you want more copper there, edit the pad properties of those holes in the footprint. There are two ways to handle this, edit directly in the board or edit the library.

  • If you edit the footprint directly in the board, then you are only editing the copy of the footprint in the board (and will be difficult to use those edits in a future board). Also if you update the footprint from the library (either manually or when updating the board from the schematic) you will permanently loose the changes unless you have a backup of the board file. This option might be fine for on-offs, but probably shouldn’t be a habit.
  • If you edit the footprint from the library you just need to remember to update the footprint on the board from the library (there is a button for this in the footprint properties in PCBNew). The complexity here is you shouldn’t save the edited footprint to the standard KiCad libraries because you would loose your changes the next time you update. (Many of the systems KiCad is installed on won’t even allow you to save to the standard libraries because they are placed in the filesystem in a place that normal user accounts aren’t allowed to write to.) The edited footprint should be put into (one of) your personal library(ies).

For the 6 board mounting holes, you have two options (listed in my personal preferred order, others on this forum reverse the preferential order, neither preference is “wrong”):

  1. As @jos mentioned in his second bullet point, four comments up, you place symbols for the mounting holes on your schematic, assign the properly sized mounting hole footprints, and then update the board from the schematic. Then move the new mounting hole footprints to where you need them on the board.
  2. Directly add the properly sized mounting hole footprint to the board using the Add footprints tool (see screenshot, below). Once you place the mounting holes where you want them you should lock the footprint just in case you need to make an edit to the schematic and re-import to the PCB. (Because the mounting holes don’t exist in the schematic, reimporting from the schematic will remove any un-locked footprint on the board that doesn’t currently exist in the schematic.)
    2020-06-23 11_04_53-Window

Hopefully you didn’t accidentally run a trace where any of the mounting holes should be. :wink:

73

Thank you @SembazuruCDE I just finished doing all of this just before your post. It took a bit of calculation etc but I think I have it all now. You guys have been brilliant helping me out with this so next one will be easier. I found the mounting holes footprint and modified it for my purpose. Then I positioned them on the board and locked them down.
I also went into my Footprint Editor and seen that the 62 pin did indeed have copper mounting rings so that is all good as well. Onward we go.

image
image1600×900 158 KB

74

Careful with those two middle mounting holes. They appear to be very close to the banana-plug socket footprints. If these are just for alignment pins, fine. But if you plan on using any type of fastener (standoff, screw, etc) make sure that you have enough space to keep your fastener from touching the socket and/or the solder pad. Especially if using metal fasteners. Also remember to leave clearance room for any tools used on the fastener, otherwise you may have trouble using the tool. (Few things are as annoying as only being able to turn a hex nut 1/6th of a turn with needle nose pliers because of a component or other feature that is in the way of a wrench or a socket driver.)

This clearance consideration is easy to overlook. Many breakout boards (and Arduinos) that I’ve seen on the market make this same mistake. Resolving issues may require design compromises.

75

Good eye. I actually caught it on my paper alignment check after that last post. My math was off and it should have had them centered between pins. All good now so i think I have everything in place. Now I just have to lay some tracks and see how that goes. Wish me luck.

76

Good luck. Your rats nests look nasty, but without re-laying out the position and/or order of all the banana sockets you may be stuck.

77

I think I am okay. I have the old one to copy from so hopefully not too much to it. We will see. I can make easy work hard lol.

78

Does this look to be correct so far?
image

image
image928×124 3.03 KB

79

The minimums are the absolute minimum that your vendor can produce at the price level that you want to order. That keeps you from accidentally specifying a track width that can’t be produced at your price level.

For the net class clearance and track width I would experiment to see the largest of both (try to keep both the same value for balance for now) and still be able to thread a track from the center row of the connector out. Be kind to your vendor and don’t immediately try to use the thinnest that they say they can produce. That will keep the amount of bad boards that they produce and have to throw away to a minimum.

80

Okay I am not sure what I have done but I can’t get rid of the markers.
Also, how do I change the trace size on all my existing paths that I have created? I started out with 6 mil and went to 12 part way through but want to go back and change the rest?

image
image596×521 26.9 KB

81

Fixed. I figured out how to change my trace width and after running DRC everything looks normal again.
How are we looking now?

image
image908×607 41.7 KB

Whats next? Ran the rules checker and checked connections.
Should I try to maximize my trace size? I printed this on paper and the traces look very small? Does it print the actual trace size or just an outline.