silkscreen Help

On 4/7/2011 11:08 AM, Matthew wrote:

Hi To All

 

I Ordered PCB From PCB Wing And I received This Error Can Anyone help Me

How To Fix it I'm New To Eagle please  I Don't Reilly Know Where Are The

Settings Of the silkscreen

 

>

Some silk screen of your PCBs are too small and their lines are

too thin to print. They'll be printed blur.

 

We recommend that they at least to be composed of 4mil thick line;

at least 25mil high, the only way they can be clearly printed.

 

>

 

Thank You !!!

Each line on the silkscreen has its own thickness.  Usually, they are

lines in parts that came fro libraries.  You have to go to each library

component and change the thickness of each line.  Also, text is drawn

from lines, so you have to increase the text ratio parameter.

On 4/7/2011 8:08 AM, Matthew wrote:

Hi To All

 

I Ordered PCB From PCB Wing And I received This Error Can Anyone help Me

How To Fix it I'm New To Eagle please  I Don't Reilly Know Where Are The

Settings Of the silkscreen

 

>

Some silk screen of your PCBs are too small and their lines are

too thin to print. They'll be printed blur.

 

We recommend that they at least to be composed of 4mil thick line;

at least 25mil high, the only way they can be clearly printed.

 

>

 

Thank You !!!

and make sure that the only font used on the board for anything,

including silkscreen, is the VECTOR font. the other fonts will look like

they work, but they can not be manufactured from the Gerber files.

On 04/07/2011 11:08 AM, Matthew wrote:

...

Some silk screen of your PCBs are too small and their lines are

too thin to print. They'll be printed blur.

 

We recommend that they at least to be composed of 4mil thick line;

at least 25mil high, the only way they can be clearly printed.

As Gary recommended, you must use the "vector" font for anything that

will wind up in a gerber file.  4 mil thick line is pretty thin for a

silkscreen.  I generally use a minimum of 7 mil.

Eagle does not directly provide a way of setting the thickness of a line

used in text.  But an /indirect/ method is available as the ration of

line width to character height.

If you want a 25mil high character, and a 5 mil line width, then you

want the ratio to be set to 5/25, or 20%.

To do this:

1) turn on the layers that will be on your silkscreen

2) Group all objects on the entire board.

3) Smash all the parts in the group.

4) change the font to vector for the group.

5) change the ratio to 20 for the group

From the command line in the board window:

    DISPLAY tOrigins tNames tPlace

    DISPLAY bOrigins bNames bPlace

    GROUP all

    SMASH (>0 0)

    CHANGE FONT vector (>0 0)

    CHANGE RATIO 20 (>0 0)

The board window shows exactly what the text will look like on the

silkscreen.  You can reposition the component names as necessary.

After producing the gerber files, it's always a good idea to use a

gerber viewer to verify correctness.  I use gerbv on linux.

Hope this helps.

Enjoy,

    - Chuck

On 04/07/2011 06:38 PM, Chuck Huber wrote:

 

If you want a 25mil high character, and a 5 mil line width, then you

want the ratio to be set to 5/25, or 20%.

 

Matthew, I forgot to include one command to set the size.  BTW, 25mil is

pretty small.  I generally use 50 mil.

From the command line in the board window:

 

    DISPLAY tOrigins tNames tPlace

    DISPLAY bOrigins bNames bPlace

    GROUP all

    SMASH (>0 0)

    CHANGE FONT vector (>0 0)

      CHANGE SIZE 25mil (>0 0)

    CHANGE RATIO 20 (>0 0)

Enjoy,

    - Chuck

On 04/07/2011 06:38 PM, Chuck Huber wrote:

 

If you want a 25mil high character, and a 5 mil line width, then you

want the ratio to be set to 5/25, or 20%.

 

Matthew, I forgot to include one command to set the size.  BTW, 25mil is

pretty small.  I generally use 50 mil.

From the command line in the board window:

 

    DISPLAY tOrigins tNames tPlace

    DISPLAY bOrigins bNames bPlace

    GROUP all

    SMASH (>0 0)

    CHANGE FONT vector (>0 0)

      CHANGE SIZE 25mil (>0 0)

    CHANGE RATIO 20 (>0 0)

Enjoy,

    - Chuck

On 4/7/2011 8:08 AM, Matthew wrote:

Hi To All

 

I Ordered PCB From PCB Wing And I received This Error Can Anyone help Me

How To Fix it I'm New To Eagle please  I Don't Reilly Know Where Are The

Settings Of the silkscreen

 

>

Some silk screen of your PCBs are too small and their lines are

too thin to print. They'll be printed blur.

 

We recommend that they at least to be composed of 4mil thick line;

at least 25mil high, the only way they can be clearly printed.

 

>

 

Thank You !!!

It's not so much of an error, as a warning. The smallest silk I ever

printed was 0.032 high with ratio of 10%. It is legible, but a little

blotchy. I used 8% ratio for some of the text and it is a little worse

than 10% ratio, but this is such a small difference that I suspect it is

coincidence. When silk gets this small, component names seem to be more

legible than longer words.

Chuck Huber wrote on Thu, 07 April 2011 18:38

Eagle does not directly provide a way of setting the thickness of a

line used in text.  But an /indirect/ method is available as the ration

of line width to character height.

Actually, it's the RATIO option of the CHANGE command.  Do HELP CHANGE.

There is one gotcha to note about RATIO though.  This got me when I first

started with Eagle.  Let's say you wanted 8mil line thickness and 75 mil

text height.  You'd expect the ratio to be 75 / 8 = 0.11.  But no that will

be way too small and the lines won't show up.  Incredibly, the RATIO

subcommand parameter is actually in percent, even though that isn't

specified anywhere!  Maybe this has been fixed in the documentation by now,

but I had to discover this by trial and error, then went back and looked

and found no mention of percent.

--

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

Thanks To All For The Help ..!!!! All Fixed 

--

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

On 4/7/11 8:08 AM, Matthew wrote:

Some silk screen of your PCBs are too small and their lines are

too thin to print. They'll be printed blur.

There are also several ULPs downloadable from CadSoft that will

go and "adjust" the width of silk-screen elements for you, so that

they meet minimum requirements.  I think the most recent one is:

   ftp://ftp.cadsoft.de/eagle/userfiles/ulp/silk_gen.ulp

(these work by copying all the graphics elements in the silkscreen

layers to a new layer.  Then when you generate gerbers you output

those new layers to the silkscreen gerber files, so it will require

a bit of a change in the gerber generation work flow as well.)

BillW