Schematic Symbols in Available Libraries and CAD Grids

[EPAIII]

I have used several PCB layout programs which also have schematic drawing facilities. Usually, but not always, the schematic symbols in the libraries provided with those programs will have been drawn with a common grid size. By that I mean that the dangling ends of the component leads or the connection points on the ends of those leads will fall on a standard grid (like 0.1" or 1mm). And if you are careful, when you create any new schematic symbols, your creations will also utilize a standard grid. This makes drawing the schematic of your project a lot easier.

But there are times when one of those standard PCB layout programs is not a good choice. One such time is the proto device I am presently working on where I plan to use Vero or strip board to make this one-off device. Among other reasons this will allow me to make revisions more easily than if I were to order actual PCBs for this. So I am using a new to me, 2D CAD program for this project: the exact one is not important but it is QCAD. I have made a blank strip board and even managed to set it up with two mirror reverse copies where parts added to one appear automatically on the other, but in mirror reverse. So I can actually see the board from both sides at the same time. And I am at the point of drawing my schematic above those two blank strip boards.

So I am searching for schematic symbol libraries that I can use with minimal editing. But the stinger is that almost every component from on-line libraries that I try does not fit on any standard grid spacing that I can set. 0.1", 0.05", 0.125", 0.0625", 1mm, 2mm - the symbols just do not fit. And what is worse is, when I try to scale the symbols so that one or several of the terminal points do fit, the others do not. And this is not the first time I have noticed this. It has existed for many years, decades, in fact.

What I am asking is, am I missing something? I thought these libraries were produced by companies that make the components. Their part footprint drawings are made to proper dimensions to reflect the actual package used. But what standards, if any do they use for the schematic symbols? What grid size, if any, do they expect them to be used with?

Or, with the multitude of these libraries on the web, am I just stuck with drawing my own, as I have been doing?

[avandalen]

I use always just Eagle PCB, the free version. Works perfect. See my website: https://avdweb.nl/

[EPAIII]

I am sure that Eagle PCB, free or paid version, is a good way to design PCBs. But I SPECIFICALLY said,

But there are times when one of those standard PCB layout programs is not a good choice.

That's NOT what I was talking about here. Your suggestion adds nothing to my knowledge.

[Andy Chee]

So I am searching for schematic symbol libraries that I can use with minimal editing. But the stinger is that almost every component from on-line libraries that I try does not fit on any standard grid spacing that I can set. 0.1", 0.05", 0.125", 0.0625", 1mm, 2mm - the symbols just do not fit.

Just to clarify, are you referring to schematic symbols used in the schematic capture?  Or are you referring to silkscreen symbols used on PCB footprints?

[abeyer]

Have you considered something like https://sourceforge.net/projects/veroroute/ that's meant for doing this? It uses a workflow more like pcb layout (and will do pcbs too) where you separate schematic from layout -- so you won't run into this issue of trying to shoehorn schematic symbols into serving for layout as well. You can even do your schematic capture in kicad and export the netlist for veroboard layout.

[jpanhalt]

But there are times when one of those standard PCB layout programs is not a good choice. One such time is the proto device I am presently working on where I plan to use Vero or strip board to make this one-off device.

At risk of useless redundancy, I  also use Eagle to layout protoboards that are based on a 0.1" grid.  I draw a schematic, then import the ratsnest into the board program and complete the layout using the same tools, with obvious modification, that are used for a regular PCB.  That gives me schematic capture and error checking.

I usually use protoboards that duplicate the typical layout of solderless breadboards, but that is not a requirement.  I created "devices" (symbol + package) for the protoboards I use most often (attached with and without grid showing).  Again, that's not required but it helps to have the VCC and GND buses shown. The symbol is simple added to the schematic in the usual way with connections made only for the two buses..

My version of Eagle allows just 2 layers (top and bottom), so I set rules for top and bottom, e.g., one is for existing  tracks and the
other is for new connections with wire.  I use a short solid bar (outline layer) for existing tracks that need to be cut. None of that is actually required.  The best part is schematic capture.

Perhaps none of this will be helpful to you.  If that's the case, you need to describe better what you are trying to do.

John

[Doctorandus_P]

I do not understand your apprehension for using a standard PCB design program.
I also do not understand your wish for schematic symbols fitting your Vero strip board.

Do you want to print your schematic, then glue it on the strip board while soldering parts to your PCB?

I also use "Vero" board, but I find the strip board abhorrent. Cutting open the strips is a nuisance, and it is also a "reverse" operation. you have to remove connections that are already there, and if you forget one, it becomes a mess.

I only use the version with one hole per island myself, and I make a part of the connections by bending the existing wires of (wired) resistors and transistors (TO92, etc) and the other connections I make with enameled wire, which you can solder directly with a hot iron. I use 0.2mm enameled wire for all connections below 300mA, and thicker wire for both power and all higher current connections.

There is specialized software for this (See Abacom / Lochmaster) but it does not run on Linux, and as far as I know it is only "drawing the PCB" only. There is no connection with a schematic.

It would have helped if you posted a few screenshots of what you do with QCad, but whether you use a mechanical CAD program or PCB design software, there is always some mismatch. I have gone the other way, and I use KiCad for all my own designs. And also use it for my one-off matrix board designs. I first draw the schematic in the normal way, then put all the footprints on the PCB, and for a one-off project on Vero board,  I use the PCB editor in such a way that the result fits on vero board. Mostly it's setting the PCB editor to a 2.54mm grid for all THT parts. If you want to use strip board, then you can easily confine yourself to only drawing horizontal tracks on one of the layers. You can even print out that layer, glue it to the PCB with water soluble glue and use it as a template for cutting the tracks. You can use the other copper layer for drawing wire bridges (you can make them all vertical if you wish).

If you want to use PCB's like the stuff with 3 holes per island, or the "Elex PCB" (see below), then you can also load them as a background image in KiCad, or you can make a template that has the same track layout in a real copper layer, and then just put your footprints on top of it. (Track names change automatically in Kicad when you put a footpint on top of it).

And you can take this concept as far as you like. For example:
1. Print the Silkscreen layer.
2. Put it on the PCB.
3. Punch holes though it with a needle.
4. Mount your parts though the holes.
5. Either leave the paper permanently (it may start conducting if it gets dirty / wet) or tear it to pieces and remove it.

For me, the advantages of using KiCad (or other dedicated PCB design program) are:
1. No extra constraints while drawing the schematic. Use labels, schematic symbols that reflect function instead of pinout etc.
2. Quite big libraries (around 20.000 parts in KiCad).
3. PCB footprints have real dimensions. (TO220 etc,) But use a few modified footprint for things like TO-92 so their pin spacing is 2.54mm.
4. ERC and DRC for error checking. (This is a big one!)
5. Because I use both the schematic and the PCB part. I can optimize the PCB part for layout on my matrix board.
6. I already know KiCad, no new software to learn.
7. Schematic parts are re-usable. (Just copy from a "standalone" instance into a project).
8. Schematic is re-usable if you decide later you do want to make a PCB of it.