se1pcb1- Simple Exercise: Dump all footprints onto drawing (PCBnew)

create counter

Go To Simple Exercise Overview Page

Go to previous page in Simple Exercise: Initial creation of NetList.

At last! Time to draw the PCB artwork!!!

This page is "dated"… the illustrations were done with a version of KiCad that is no longer (12/19) current. But the essence now is as it was then. Yes, some of KiCad's rough edges have been smoothed. New tools are available. But in 12/19, I loaded KiCad 5-1-5 onto a previously KiCad-less Windows 10 machine, and went through this "Start Here"/ "Simple Introductory Exercise" tutorial, and it was still pretty much on target.

Here… more or less… is what the finished design looked like "in the olden time". (I tweaked the colors a bit)….

And here is what the finished design looked like under ver 5-1-5…

(In both cases, the green lines are the copper tracks… rather thinner than you will make them, once you have mastered KiCad, and very crudely laid out. But they would do as a first effort, wouldn't they? Learn to "walk" before you try to "run"!)

Carrying on from where we got to previously, we would…

Launch PCBnew. (Later you will use it for editing earlier work, too, by the way… it is not just for "new" boards, despite the name. I think the program was a replacement for an older program, somewhere in KiCad's history.)

As with CVpcb, you can use the central project manager window, or the button on the tool bar at the top of eeSchema….

If you're running an old version of KiCad, the first time you do this, you may get the warning which will become familiar to you, as it arises in several place in the design cycle…

Say "OK". By the way: You don't need to use "File | New" (or the "New Board" button).

Use the icon on the top toolbar to read the netlist. (Same icon as in the other modules, as you would expect… KiCad really is well put together… even if, to a novice, some things aren't intuitive. The more I use it, the more I realize that "faults" in it were merely my lack of understanding.)

At 7/14, the icon was the word "Net" with a wrench coming in from lower right… it may be "hidden", if your window is not wide enough. The somewhat unclear "Netlist" item in the "Tools" menu will do the same thing. By 1/17, vers 4-0-4 the icon had "Net" on a green background beneath what looks like an "x", but is probably meant to be tracks.

That used to bring up something like…

… and now (1/17, ver 4-0-4) brings up…

See how KiCad is evolving, improving.

By the way: The "Filter All" tickbox at the bottom? Ticking it doesn't PREVENT all messages, warnings, etc from getting through. I suppose the author would argue he/ she meant "setting the filter to all means report all messages, etc." Maybe "Show" instead of "filter", next time? Quibble? Moi?)

What we're trying to do…

At the moment, we just want to read the netlist we created in the previous step into PcbNew. We don't need to mess with the radio buttons. "Just" get the right string in the "Netlist File" edit box… it may be there when the dialog opens… and click "Read Current Netlist". Don't be too quick to assume "nothing happened."

PCB layout, here we come…

If all went well, we now have a "heap" of footprints somewhere on the PcbNew "page". In the old days, they were on the area just above and left of the upper left hand corner of the main work area. It won't look exactly like the following, but that should reveal something a bit like….

"In the old days"….

What we have is a working area. It has the red "legend" drawn around it, with some useful information filled into the boxes at the lower right. At the upper left, just outside the legends red box, we have all of footprints, in an unhelpful heap! It is like starting a jigsaw puzzle. All the pieces are in a higglety- pigglety pile. The bad news is that we now have to sort them out. The good news is that we do have all of the pieces, and "all" we have to do is sort them out and connect them up. We even get help with the connecting!

You will have to zoom and pan to see the things shown above. The gray band marks where I have "spliced" two parts of the overall workspace down into a smaller image. Even so, there is too much here to see everything clearly… but I think (tell me!) it suffices. On our machine if you zoom and pan to the lower right, you will, I hope, see the red lines, boxes and text of the drawings "legend". (See why we put a version ID into the file name? The file name appears in the legend.)

At 1/17, vers 4-0-4, with very little zoom, so you can see "the big picture", this is what you have after reading the netlist…

… and here's what is at the center of that… all the footprints in a heap.

There are all sorts of things to learn about dragging things around, and I don't want this "introduction" to drag out to 50 pages.

Even so, I do need you to go off and look at "a detail" of operating PcbNew at this point. Open this link to information about the "Mode Footprint" button in a new tab or window. Read what's there. Close the new tab… and you should find yourself back here, ready to go onward…


First, "untangle" the "heap" a bit. Either use the idea presented in the page I sent you to, or…

Make sure that the "pointer" button in the right hand tool bar is selected.

Put the cursor over the heap, press "M". (If you get a "selection clarification" dialog, be sure to select a footprint.) Move the mouse… one of the footprints should move. When it is clear of the rest, click, to "drop" it where you've dragged it.

If you find yourself moving not a whole footprint, but just some of the text that goes with it, press the "escape" key to cancel the flawed move attempt. Eventually you will WANT to move just the reference text, or value text… but we don't need to talk about… or do… that now.

When you've got the heap somewhat untangled, refine the placement of the footprints, until you have something close to one of the following…

Here's where we would have been before Kicad version 4, with the footprints chosen when this tutorial was new…

… and here's where we would be, if we were following the 12/19 update of the tutorial, to bring it in line with KiCad 5-1-5…

… down in the lower right of the "frame", just about the legend. (Press "R" as needed to rotate footprints to the right orientation.) (Any time you have a footprint (module) "stuck" to the cursor, you can rotate it, by pressing "R".)

The white lines, by the way, are not, exactly, the tracks of the design. The are the circuit rats nest. More on them in the next page.

Something you might have noticed:

If you have the pointer button of the right hand tool bar selected, as you should, and you move over something, and then press M, that's all you have to do to pick it up.

In most Windows applications, if you wanted to move, say, the switch's footprint, you would move over it, click the mouse to select the footprint and then press "M" and start moving the object.

The KiCad approach takes a bit of getting used to, but is wonderful when you have made the transition.

(What is not so wonderful is, while writing this for you, switching back and forth between KiCad and the graphics editor I use… which has a more traditional interface. It doesn't help that I am working with nearly the same image in the two applications, but with it responding differently in each!!)

And another thing….

Just one more little aside before we finish this page:

You need to know that for most of the time you are working, you will be looking at the "front" of the PCB. If you are doing a simple single sided board, the tracks will be on the "back" side of the board.

While on the computer, dealing with the "virtual" PCB, you will be viewing it from the front, with "X-ray eyes". (Or, to put it a little less dramatically, you are viewing it as if the insulating substance of the board is transparent…. glass, not fiber-glass or phenolic cotton paper!)

If you are going to prepare the actual PCB "by hand", you simply tick the "mirror" box on the "print dialog to get the printout of the artwork "flipped over", so that it looks like what you should see when looking at the "back" side of the board… where the "first" collection of tracks goes. (Speaking of the "print" dialog, be sure to tick "single page", too… and remember that it, rather annoyingly, isn't "sticky". Many of the other "print" dialog selections are sticky, just to add to the chances of going wrong!)

Go to next page in Simple Exercise: Placing tracks on PCB design.

Go to main page of

Unless otherwise stated, the content of this page is licensed under Creative Commons Attribution-ShareAlike 3.0 License