EDAboard.com | EDAboard.de | EDAboard.co.uk | WTWH Media

tiny silkscreen

Ask a question - edaboard.com

elektroda.net NewsGroups Forum Index - Electronics Design - tiny silkscreen

John Larkin
Guest

Sun Feb 10, 2019 9:45 pm   



I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.



--

John Larkin Highland Technology, Inc

lunatic fringe electronics

Uwe Bonnes
Guest

Sun Feb 10, 2019 10:45 pm   



John Larkin <jjlarkin_at_highlandtechnology.com> wrote:
Quote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.

Most device name I do with 0.8 mm high font and a linewidth of 0.16 mm.
There are readable.
--
Uwe Bonnes bon_at_elektron.ikp.physik.tu-darmstadt.de

Institut fuer Kernphysik Schlossgartenstrasse 9 64289 Darmstadt
--------- Tel. 06151 1623569 ------- Fax. 06151 1623305 ---------

Winfield Hill
Guest

Sun Feb 10, 2019 10:45 pm   



John Larkin wrote...
Quote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.


I often do 40 mil character height, 10 mil width.
Parts that are crammed, get 38 - 8, or 37 - 7
Comes out fine on the PCB, could go down more.

Last design, skipped 40 - 10, except some ICs.


--
Thanks,
- Win

Winfield Hill
Guest

Sun Feb 10, 2019 11:45 pm   



Winfield Hill wrote...
Quote:

Uwe Bonnes wrote...

John Larkin <jjlarkin_at_highlandtechnology.com> wrote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

Most device name I do with 0.8 mm high font and a linewidth of 0.16 mm.
There are readable.

I haven't been that brave yet. But I have done boards
without any part designators, or only the ICs, etc.
Forces users to have a parts-location drawing handy.


Many of my boards use 0805 parts and have expanded
footprints to make hand assembly easier. For this
case, space taken for part designators isn't bad.
But with 0603 parts it begins to get unreasonable.
And for smaller sizes, forget it!

I've seen high-volume boards with parts-designator
info around the edges, tightly packed and lined up
with the part-location order. That works well.
Often you really need parts immediately adjacent,
removing the designators to the edge can help.


--
Thanks,
- Win

Winfield Hill
Guest

Sun Feb 10, 2019 11:45 pm   



Uwe Bonnes wrote...
Quote:

John Larkin <jjlarkin_at_highlandtechnology.com> wrote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

Most device name I do with 0.8 mm high font and a linewidth of 0.16 mm.
There are readable.


I haven't been that brave yet. But I have done boards
without any part designators, or only the ICs, etc.
Forces users to have a parts-location drawing handy.


--
Thanks,
- Win

David Nadlinger
Guest

Mon Feb 11, 2019 1:45 am   



On 10.02.19 8:06 PM, John Larkin wrote:
> What's the smallest silk that anyone has done successfully?

26 mil font height/4 mil stroke width, with the default Altium stroke font.

This was for a quick prototype board ordered off SeeedStudio, and the
designators came back perfectly readable.

— David

speff
Guest

Mon Feb 11, 2019 1:45 am   



On Sunday, 10 February 2019 15:06:42 UTC-5, John Larkin wrote:
Quote:
I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.

0.6mm with 0.18mm stroke is what I usually use these days on tight boards, more like 1mm with 0.2mm stroke on less tight boards. Usually comes out okay.


40 mils is about 1mm, of course. I think you should be fine.

--Spehro Pefhany

Lasse Langwadt Christense
Guest

Mon Feb 11, 2019 1:45 am   



mandag den 11. februar 2019 kl. 00.52.54 UTC+1 skrev John Larkin:
Quote:
On 10 Feb 2019 14:23:01 -0800, Winfield Hill
hill_at_rowland.harvard.edu> wrote:

Winfield Hill wrote...

Uwe Bonnes wrote...

John Larkin <jjlarkin_at_highlandtechnology.com> wrote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

Most device name I do with 0.8 mm high font and a linewidth of 0.16 mm.
There are readable.

Yikes, that's 32 mils in American units! I felt brave considering 45.


this guy show some examples made by OSH Park

https://lukemiller.org/index.php/2015/07/pcb-silkscreen-sizes/

John Larkin
Guest

Mon Feb 11, 2019 1:45 am   



On 10 Feb 2019 14:23:01 -0800, Winfield Hill
<hill_at_rowland.harvard.edu> wrote:

Quote:
Winfield Hill wrote...

Uwe Bonnes wrote...

John Larkin <jjlarkin_at_highlandtechnology.com> wrote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

Most device name I do with 0.8 mm high font and a linewidth of 0.16 mm.
There are readable.


Yikes, that's 32 mils in American units! I felt brave considering 45.

Quote:

I haven't been that brave yet. But I have done boards
without any part designators, or only the ICs, etc.
Forces users to have a parts-location drawing handy.

Many of my boards use 0805 parts and have expanded
footprints to make hand assembly easier. For this
case, space taken for part designators isn't bad.
But with 0603 parts it begins to get unreasonable.
And for smaller sizes, forget it!


I like 0805s usually, but this board is about as big as a postage
stamp (a little less, actually) and is 0603s and some microscopic EPC
fets.

The EPC parts are hard to place and hard to rework, and fragile, so
I'm putting them on what I hope is a common sub-assembly that we can
make in quantity. It becomes a component for a bigger board. If a GaN
fet fails, we'll just replace the entire baby board.

It will be a mouse-bite thing like this

https://www.dropbox.com/s/mw2j725qshitdrh/T852B_Glob_1.JPG?dl=0

https://www.dropbox.com/s/93cuoljq6z8z9yc/DSC02362.JPG?dl=0

but will have a lot of parts.

My manufacturing people like ref desigs, but they'd need to be really
small.


--

John Larkin Highland Technology, Inc

lunatic fringe electronics

Tim Williams
Guest

Mon Feb 11, 2019 2:45 am   



Did 25 mil height, 4 mil linewidth with fab Eagle Electronics, came out just
legible (if you don't mind that it's that small; poor eyes need a magnifier
for sure).

I don't think even the cheap Chinese proto fabs have a problem with 30/6 mil
text.

I have 30/6 set as default.

Tim

--
Seven Transistor Labs, LLC
Electrical Engineering Consultation and Design
Website: https://www.seventransistorlabs.com/

"John Larkin" <jjlarkin_at_highlandtechnology.com> wrote in message
news:up016edlscer3j31cpfb0ej5qopgcu9j5m_at_4ax.com...
Quote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.



--

John Larkin Highland Technology, Inc

lunatic fringe electronics


Jasen Betts
Guest

Mon Feb 11, 2019 5:45 am   



On 2019-02-10, John Larkin <jjlarkin_at_highlandtechnology.com> wrote:
Quote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?


my Digi-Key ruler has legible 20mil writing.

--
When I tried casting out nines I made a hash of it.

Robert Baer
Guest

Tue Feb 12, 2019 1:45 am   



John Larkin wrote:
Quote:

I'm fiddling with a tiny PCB layout (to avoid some other chores) and
trying to decide if I want component silkscreens, outlines and ref
designators. They would have to be 50 mils high, preferred only 40.

What's the smallest silk that anyone has done successfully?

I'll verify with our PCB vendors tomorrow.



4 mil vector graphics seem to be rather reliable.


elektroda.net NewsGroups Forum Index - Electronics Design - tiny silkscreen

Ask a question - edaboard.com

Arabic version Bulgarian version Catalan version Czech version Danish version German version Greek version English version Spanish version Finnish version French version Hindi version Croatian version Indonesian version Italian version Hebrew version Japanese version Korean version Lithuanian version Latvian version Dutch version Norwegian version Polish version Portuguese version Romanian version Russian version Slovak version Slovenian version Serbian version Swedish version Tagalog version Ukrainian version Vietnamese version Chinese version Turkish version
EDAboard.com map