Guidelines for Schematic & Symbols Design (Projects & Libraries)

Hello Folks,

I am begining a new project and I would like to use common Schematic design guidelines (which must not to be the same as PCB Layout guidelines). So, I wonder if you could help me with some advice.

Anyway, to begin the discussion, I have some questions already. For instance:

1) Which is the best Grid size when you design Schematic Symbols and aftewords, which is the best Grid size when you begin to draw the Schematic itself using those symbols?

This question rises because if for instance I choose a very small grid (for instance 0.001mm), then it is very difficult to pick-&-point with accuracy. So, I want to choose the best grid size, and always use it as reference for new projects and symbols. (Maybe 1mm? :-|)

2) Which is the best recommendation to create new electronic symbols?

I found this link:
Electronic symbol - Wikipedia, the free encyclopedia

But I don't know if there is any other free electronic Standard available.

3) Is better to draw the symbols for the libraries: Horizontally or Vertically? :roll:

a) or b)



Thanks a lot in advance by your wise and support! ;-)

Look for IEEE- Std 315 and or ANSI Y32.2. These are the drawing and reference designator standards.

I use the default Grid size that comes with my package. It is 0.25mm.

1) But the standard for schematic symbols is not the IPC-2612? Are any free available standards?

2) Why do you use 0.25mm and not 1mm? Or if if want smaller, why not 0.1mm? (Then, you could increase/decrease the grid size in 10x factors)

What package are you using? All packages have standard symbols based on a particular grid, often 0.1". Stick to that. If you start using fine grids for the pins you will end up with all sorts of connection problems - connections which look like they are made but aren't.

It doesn't matter whether you draw the standard components vertically or horizontally - it should be a single key stroke to rotate them. Items like a diode should be a standard part of the software anyway.

Keith.

I use Altium. You can switch grids as you go along. My pin one is always top and/or left.
IPC-2612 is another standard. Most of it is the same as IEEE. IEEE and IPC are all copyrighted material. So you will need to buy them.

I use IPC-2612, it is a combination of the other standards that have been used over the years. It provides a good basis for your schematic standards.
As to your grid size, its way to small for schematics. I started out drawing them by pen using a drawing board (pre schematic capture package days!) and used the old BS-308 mechanical drafting standard as a basis for line widths then. What you have to determine is how the schematcis will look when printed and paper sizes. As a reccomendation that I know works and can be printed 1 sheet size smaller and still be legible is:
2.5mm - 3mm between IC terminals, discrete component symbols (res, caps, diodes etc) 7.5mm between symbols, pin text and signal names 1.75-2mm high. Space connections at 2.5-3.0mm apart to match IC pins spacing. Base you design grid on the pin to pin spacing again 2.5-3.0mm and only use the desig grid and half grids for design to keep things tidy. On all ECAD systems you can define macros to set the grids and have these on a custom tool bar or as a custom keyboard shortcut.
The IPC- specs cost very little, buying them helps support the organisation, and the cost is offset by the time you save having to do your own specs.
With regards to bolth schematic symbols and component footprints, the first thing I do with any CAD package is delete the ones that come with them and do my own, not only does it teach you the most important basic skill of CAD, LIBRARY MANAGEMENT, but it gives you complete control of what you do, what is displayed and any extra information you want to include.

I use Altium and CadStar. From your advices, maybe 0.5mm could be a good grid size.

My colleagues are using 1.5mm, but I think that it is not a good idea because it is difficult to make smaller factors:

1,5mm => 0.75mm => 0.375mm

But:

0,5mm seems a good factor.

What do you think? :-|

0.5mm for what?

I hope you are not talking about having 0.5mm between symbol terminals?

Consider the size of text for signal names, pin no's and pin labels, it will have to be so small that it will be illegible.

A schematic should look clear and easily readable when printed so that can include the need to ensure that your line/text widths are of a reasonable size to display well. If you have an old photocopier (as most places do) that you have to use for your printer you are limited to A4/A3, however making
the schematic with fine lines, small distances between everything and very small text will make for a schematic that requires a magnifying glass for us old farts to read.

IC's are getting higher pin counts so there can be more to cram into a schematic, however you still do not need to use a very fine terminal pitch
as you can split most large IC's into many gates so that you can draw a schematic with good schematic flow that reads well.

I have tried using 1mm pitch between pins and it was awful, you could hardly tell which pin a text or pin no was referring to.

The old symbols that use a 0.1" grid and 0.6" between resistor terminals did not choose that value just for fun.

By the way, there is no real reason why you MUST use a metric grid for schematic symbols/circuit diagrams. They do not have to be on any metric based pitch at all, PCB's maybe - schematics do not need it.

When I draw a schematic I put supply rails at top and bottom. Positive at top.

All the action takes place in between. Current flow predominantly downward.

The custom is to show signal/information flow going from left to right. Input at left. Output at right.

Devices which drop DC voltage make sense when oriented vertically. So that the trend of current flow is downward.

Other devices which don't carry DC power, or which oscillate (capacitors, coils), make sense oriented horizontally.

When drawing an IC I locate the pins where the shortest line can be drawn to whatever they're connected to.

Not hard and fast rules. Just guidelines to make it easy for the reader to grasp what's going on.

I see, so maybe 1mm or 1.5mm as grid for my schematics and schematics symbols should be fine.

I'll dig out a couple of Cadstar examples later, and again re-iterate that you have to cater for printing out the schematics when creating the symbols, page borders etc.

I see Marce, I will wait your later reply. By the way, do you work with CadStar daily? Do you know well the tool?

I think the answer will certainly be yes to that one :-D

Why don't you try digging out existing standards and seeing what they say?

Sorry haven't replied in detail, been in meetings all day!!!
Cheers Matt, between us we probably have getting on for half a centuary's experience, I've used it for 25 years.

I'm only a noob compared to Marc - 15 years, Marc wrote the book and I'm reading it to other...lol

There are standards for symbols, in the UK there are old and new standards available - however for basic symbols, D/C/R they are pretty basic and used by many - ANSI is an old standard however it is what many of us grew up with and also what is still often used in learning as the tutor learnt using it themselves.

Most symbols are covered in very similar ways by the various standards, adding to that consider things like how it will be viewed, printed and its effect on giving the viewer the correct impression of what it is doing.

Many companies have their own take on what symbols should look like.

What is it about the existing standards you have found that you do not like?

I had not access to the standards because they are not free available. And my group cannot afford its purchase.

the delay, been rather busy.
Attached is a Cadstar csa file (just read it in to create a new schematic), with some examples of symbols and a A3 border, these are all designed to be printed out at etwo scale factors, 1 and 0.707.
I have added some discretes and a few chips so you can see the relationship between the symbols and text sizes etc.
When designing these sort of things you are best not to go below a font size of 6 points, this equates to a capitol H character size of 1.5 to 1.8mm depending on typeface, though 8 point is better (1.8 - 2.0mm H height).
Digest this data and let us know if you have any more questions.

Marce
Well, you have designed your schematic symbols with a 0.25mm grid, which I think is a bit small to work, isn't? By the way, I agree that working with 1mm grid is maybe the better smaller size grid to take into account.

No the basic grid for these symblos is 5mm, that is the distance between the pins and thus determines the grid you can use for your system grid when designing a schematic, for these symbols I would use a working grid of 2.5 or 5mm. Change the grid to 5mm and add some connections, you will understand what I mean then. Ignore the grid it loaded at, I set this file up from some old data I had at home (I have libaraies going back many many years that I have developed, I keep the old version for historical purposes).
All the symbols connecting points are based on a distance of 5mm, thus giving the working grid, as stated earlier, try adding some connections and moving symbols with this grid spacing and then report back.
When I design the symbols I use a smaller grid to get the detail in, but when read into the schematic the working grid is 5 or 2.5mm...

Yes, I see, it is quite confortable to work with 2.5 or even 5mm. So, if I undertood well, did you design the symbols maybe with 1mm working grid and 5mm visible grid; and afterwords you draw the schematics with 5mm working grid? Cool! :grin: