best text size?

Font size 12 is best. 10 may use for compact.

Also, is there any way to go thru a whole library and change text size, or do I need to look them one by one?

12? Do you mean a ratio of 12?  What size?

12 pt. Ref - MS OFFICE

d b wrote on Fri, 22 June 2012 21:25

I am making components for libraires, but I don't want all different

font sizes as I use my custom ones and the standard ones.

 

What is the most common size so I can try to match as I make mine?

For schematics and symbols, 0.07" is best since it can be centered in the

standard 0.1" grid.

For pcb and footprints, I find that 0.8mm in the vector font and ration of

15% is the smallest that I can get to be reproducible across a bunch of

different manufacturers.  If you're using a more advanced PCB process you

can usually get to 0.6mm.  Always use the vector font in the PCB.  If you

use Proportional font then the size can change between the screen and the

gerbers.

Now my designs are usually dense so I try to get the smallest.  For sparser

designs I use 1mm size and that seems pretty good.  It really depends on

your design and how small you can read

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Thanks

I have all editors set to inches.

Do you mean .07 *inches* for schematic but metric .8 *mm* for footprints?

Rigth now I'm set to .05 inches and 10% for foorptints. Possibly way too big from what you are saying.

d b wrote on Mon, 02 July 2012 02:45

Thanks

I have all editors set to inches.

 

Do you mean .07 inches for schematic but metric .8 mm for

footprints?

 

Rigth now I'm set to .05 inches and 10% for foorptints. Possibly way

too big from what you are saying.

A standard CAD Schematic (at least here in North America) is always in

0.1"-grid, not just in EAGLE.  So I stick with that.

But PCB can be anything you like and I prefer metric.  But obviously you

could convert that to inches if you'd like.

I was giving the smallest, you can make it bigger at will.  When silk gets

too small then parts of the text will either blob or thinned out too much.

But big isn't a problem.  I find 1mm to be a good size but others may have

different opinions.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

It's not an issue for routing to have most parts packages sized for .100 grid, and then plaved in a metric grid?

Hi,

Your objectives are to make silkscreen text printable and readable.

Check with your board house what minimum silkscreen width they can

reliably print.  Olimex, for example, specify 10mil (0.254mm), other

board houses give a figure of 8mil or sometimes 5mil.

You will then need to choose a text size that is comfortable to read

when assembling/debugging boards.  I go for 50mil (1.27mm) but this is

quite large.  The best way to find out what works is to print a

life-sized copy of the silkscreen layer.

To meet the silkscreen width requirement of your board house you will

need a suitable "Ratio" setting.  I use 20% which, for 50mil text, gives

10mil thickness.

You will see that most of the EAGLE standard libraries use 50mil text

and either 8% or 10% ratio, giving rather feeble 4mil and 5mil

silkscreen widths respectively.  Some board houses will struggle to

print these.  When I use standard parts, I usually "SMASH" them and

change the ratio of "tNames"-layer text to 20%*.

For non-silkscreen drawings or text (e.g. "tValues" and "tDocu" which

are generally not printed on the PCB), which are used to produce

assembly/test documentation, you have much more freedom.

In schematic symbols, 0.07 inch text (with 8% ratio) is standard.

In a thread on "eagle.userchat.eng" in November last year, Jeorge Garcia

of Cadsoft proposed a set of standards for libraries.  I'd be interested

to see if this took off.

Andrew

0xADF

• display none tOrigins bOrigins; group all; smash (>0 0); display last;

display none tNames bNames; group all; change size 50mil (>0 0); change

ratio 20; display last

On 23/06/2012 02:25, d r wrote:

I am making components for libraires, but I don't want all different font sizes as I use my custom ones and the standard ones.

 

What is the most common size so I can try to match as I make mine?

 

Thanks very much.

I'm going to use 50mil and 10% and propose that becomes the standard.