← Back to team overview

kicad-developers team mailing list archive

Re: Silk screen line width behavior.


Le 09/11/2010 22:30, Wayne Stambaugh a écrit :

On 11/9/2010 4:11 PM, Dick Hollenbeck wrote:
On 11/09/2010 02:35 PM, Wayne Stambaugh wrote:
I just got DFM failure from my PCB manufacture for silk screen width of 0.001"
for all the silk screen drawings on a board I just laid out.  I checked all of
the module silk screen widths and everything is 0.005" or larger.  A quick
check of the silk screen layer gerber file revealed the aperture being used was
indeed 0.001".  After some digging around, I found that changing the "Default
pen size" in the plot dialog changed the silk screen line width.  Is this the
appropriate behavior?  Setting the default line width to 0 did not fall back to
the line width defined in the module.  I would expect my silk screen line
widths to be what I defined them in my module not the default pen size setting.
  At one time, I thought this was the default behavior.  Before I file a bug
report, I wanted to make sure I'm not missing something.  Anyone else have any
thoughts on this?


Its not perfectly pertinent to your question, but I have found


to be useful after I have a board ready to plot.

I have not stumbled onto your problem before.  Maybe something has
changed, or I just missed it.

I haven't laid out a board with the latest stable version so I can't say for
sure but I don't remember having this problem with the previous stable version.

> From a UI perspective, I would not prefer to have to set the default
width to zero to say, "leave me alone".

I would prefer to select a checkbox saying override the line-widths, or NOT.

A check box would be preferable.  Setting the line width to 0 is less than
obvious to the user.  Currently, setting the line width to 0 will set the
aperture to 0 which in itself might be consider a bug.  I confirmed this with
BZR 2595.



Default pen size is used *only* to plot items that have no line width specified.
	sheet references (if asked, not usual in gerber files)
	and pads in sketch mode on silk screen.
Silk screen layers are the 2 layers that do not use filled shapes to show pads, when they are put on these layers.
So they use the default pen to plot pads.

Other items must be drawn with their own line width, regardless the default pen size.

An other behavior is a bug.
So no need to have a check box.

I am unable to reproduce your problem on my boards (just pads on silkscreen layers use the default pen).

Jean-Pierre CHARRAS

Follow ups