Gerber Silkscreen Bug?


#1

Hi,

I have this layout in PCBnew http://prntscr.com/fisbgf

However, when I create the Gerbers I get this:

There are huge generated top silkscreen noise/lines … The only thing different with this project as opposed to the many other successful boards is that I have been importing dxf graphics onto the top silkscreen … so I suspect it is something to do with that, but I cannot see the lines to remove them in PCBnew?

Any thoughts or things to try?

Regards,
Tom


#2

It would help to post the gerbers. What gerber viewer are you using?


#3

What paper size is this in the background of the layout?

You won’t be able to zoom that far out in PCBnew, to delete the dxf stuff manually.
You have to do that in a text editor…

PS: you could try to use A1 or whatever the biggest size is that is available (or can be set up) and see if you can get out there.


#4

This result looks similar to the integer overflow bug we had a while back.
https://bugs.launchpad.net/kicad/+bug/1661705

How does it look in the 3d viewer?

You can try exporting in gerber 4.5 (for some reasone gerber 4.5 did not suffer from the integer overflow bug.)

But as others have said, there must be some feature on silk this far out. maybe there is some graphics element in one of the far corners.


#5

@Joan_Sparky - I have increased the size of the page to A1 see here, http://prntscr.com/fit8fs, but this has not helped, in fact I now have some weird misalignment with the top silkscreen and the rest of the board in when the Gerbers are generated, see here - http://prntscr.com/fit98f

@Rene_Poschl - I have tried in 4.5mm instead of 4.6mm and I get the same problem. In fact the Gerber view in the link above is in 4.5mm.

(@)bobc I would prefer not to post the Gerbers since this is for a commercial project.

I would guess that the number of lines shown are equal to the number of times I have imported a DXF into this design … I have tried rebuilding from the net, but they persist.

Regards,
Tom


#6

Ok, no problem. I think the DXF might be a red herring, it does look more like the text bug @Rene_Poschl refers to. Not sure best way to fix it, but looking at the kicad_pcb file in a text editor should quickly show the problem. If you search for “gr_text” you should find lines like

(gr_text “LED Driver” (at 120 111 90) (layer F.SilkS)

If the coordinates are ridiculous, then it’s the “text bug”.


#7

Did you try to zoom out with that large sheet?
I was just assuming that PCBnew would let you go ‘out there’ if the sheet was bigger, so you could delete the wrong stuff.

That failing… open the [project].kicad_pcb file in a text editor (notepad++ under Windows is a good one) and locate something like this (bold stuff is the important one):

(gr_line (start 165.5 95.25) (end 147.75 115.25) (angle 90) (layer F.SilkS) (width 0.2))

Look out for VERY LARGE start/end coordinates.
Delete those lines.
If there had been arcs their lines will be in that area of the file as well…

PS: make a copy of the whole project folder before you do this.


#8

I investigated the kicad_pcb file in notepad++ and was exicited to see when I searched gr_line a large block of high values, here https://prnt.sc/fitmex

I deleted them and reloaded the project and rebuilt the Gerbers, but the lines were still there. I went back to double check that the gr_line were deleted and they were, but somehow they remain in the Gerbers …?

I have pasted the gerber contents here (sorry but as new user I am not allowed to upload files!). I cannot see any whacky co-ords in this file?


#9

This block is causing the lines, if you delete it the file looks ok:

D13*
X2144650995Y-2045930685D02*
X2144650995Y2131904059D01*
X-2113944095Y2131904059D01*
X2138985690Y-2060093948D01*
X-2074739236Y2133320385D01*
X2096948178Y2134736711D01*
X2096948178Y-2055844969D01*
X-2074739236Y-2054428643D01*
X2138985690Y2138985690D01*
X-2113944095Y-2053012316D01*
X2144650995Y-2053012316D01*
X-2041199683Y-2045930685D02*
X-1999162171Y2146067322D01*
X-2080404542Y2144650995D01*
X-2080404542Y2131904059D01*
X-2091735152Y-2045930685D02*
X-2091735152Y2138985690D01*
X-1968455271Y2137569364D01*
X-1926417759Y-2055844969D01*
X-2046864988Y-2055844969D01*
X-2004827477Y2137569364D01*
X-2091735152Y2146067322D02*
X-2049697641Y-2045930685D01*
X-2046864988Y-2045930685D01*
X-2004827477Y2146067322D01*
X-2086069847Y2144650995D01*
X-2086069847Y2143234669D01*
X-2004827477Y2141818343D01*
X-2046864988Y-2051595990D01*
X-2049697641Y-2051595990D01*
X-2091735152Y2140402017D01*
X-2136605317Y-2055844969D02*
X-2100233110Y-2055844969D01*
X-2097400458Y2131904059D02*
X-2097400458Y2144650995D01*
X-2016158087Y2146067322D01*
X-2058195599Y-2045930685D01*
X-2100233110Y-2045930685D01*
X2110659162Y-2055844969D02*
X2147031369Y-2055844969D01*
X-2145103275Y-2045930685D02*
X-2145103275Y-2058677622D01*
X-2063860904Y-2060093948D01*
X-2105898416Y2131904059D01*
X2147031369Y2131904059D01*
X2141366063Y-2045930685D02*
X-2111563721Y2146067322D01*
X2102161204Y-2047347011D01*
X2020918834Y-2048763338D01*
X2020918834Y-2053012316D01*
X2102161204Y-2054428643D01*
X-2111563721Y2137569364D01*
X2141366063Y-2055844969D01*
X-2114396374Y-2055844969D01*
X2138533410Y2137569364D01*
X2015253529Y-2054428643D01*
X2096495899Y-2053012316D01*
X2096495899Y-2048763338D01*
X2015253529Y-2047347011D01*
X2138533410Y2146067322D01*
X-2114396374Y-2045930685D01*
X2141366063Y-2045930685D01*
X2009588223Y-2045930685D02*
X2009588223Y-2055844969D01*
X2009588223Y-2053012316D02*
X2090830594Y-2054428643D01*
X1967550712Y2137569364D01*
X1925513200Y-2055844969D01*
X2087997941Y-2055844969D01*
X2043127776Y-2045930685D02*
X2043127776Y-2055844969D01*
X2043127776Y-2054428643D02*
X2124370147Y2137569364D01*
X2082332635Y-2055844969D01*
X2121537494Y-2055844969D01*
X2079499982Y2137569364D01*
X1956220101Y2138985690D01*
X1956220101Y-2045930685D01*
X1956220101Y2138985690D02*
X2037462471Y2137569364D01*
X1995424959Y-2055844969D01*
X2034629818Y-2055844969D01*
X1992592307Y2137569364D01*
X2073834677Y2138985690D01*
X2073834677Y-2045930685D01*
X2140913783Y-2045930685D02*
X2140913783Y2131904059D01*
X2093210966Y-2045930685D02*
X-2114848654Y-2054428643D01*
X2093210966Y2131904059D02*
X2140913783Y2140402017D01*
X-2084141754Y-2045930685D02*
X-2084141754Y-2055844969D01*
X-2084141754Y2131904059D02*
X2129583172Y-2060093948D01*
X-2084141754Y2133320385D01*
X-2002899383Y-2060093948D01*
X-2084141754Y2131904059D01*
X-2084141754Y2133320385D01*
X-2089807059Y-2055844969D02*
X-2089807059Y-2045930685D01*
X-2089807059Y-2054428643D02*
X-2008564688Y2137569364D01*
X-2050602200Y-2055844969D01*
X-2011397341Y-2055844969D01*
X-2053434853Y2137569364D01*
X2118252562Y2138985690D01*
X2118252562Y-2045930685D01*
X-2146007834Y2146067322D02*
X-2103970322Y-2045930685D01*
X2070549745Y-2045930685D01*
X2112587256Y2146067322D01*
X2031344886Y2144650995D01*
X2031344886Y2138985690D01*
X2112587256Y2137569364D01*
X2070549745Y-2055844969D01*
X-2103970322Y-2055844969D01*
X-2146007834Y2137569364D01*
X2025679581Y2138985690D01*
X2025679581Y2140402017D01*
X2031344886Y2141818343D01*
X2104089298Y-2055844969D02*
X2140461505Y-2055844969D01*
X2143294157Y2131904059D02*
X2143294157Y2144650995D01*
X-2070430768Y2146067322D01*
X-2112468280Y-2045930685D01*
X2140461505Y-2045930685D01*
X2095591340Y-2045930685D02*
X2095591340Y-2055844969D01*
X2095591340Y2131904059D02*
X2014348970Y-2060093948D01*
X2095591340Y2133320385D01*
X-2118133585Y-2060093948D01*
X2095591340Y2131904059D01*
X2095591340Y2133320385D01*
X2003018360Y2146067322D02*
X2045055871Y-2045930685D01*
X2129130894Y-2045930685D01*
X-2123798890Y2146067322D01*
X2089926035Y-2047347011D01*
X2008683665Y-2048763338D01*
X2008683665Y-2053012316D01*
X2089926035Y-2054428643D01*
X-2123798890Y2137569364D01*
X2129130894Y-2055844969D01*
X2045055871Y-2055844969D01*
X2003018360Y2137569364D01*
X2039390566Y2146067322D02*
X-2093091989Y-2045930685D01*
X2117800284Y-2045930685D01*
X2075762772Y2146067322D01*
X-2137962154Y2144650995D01*
X-2137962154Y-2048763338D01*
X2075762772Y-2050179664D01*
X2117800284Y2141818343D01*
X2078595425Y2141818343D01*
X2120632936Y-2051595990D01*
X2039390566Y-2053012316D01*
X2039390566Y2138985690D01*
X2120632936Y2137569364D01*
X2078595425Y-2055844969D01*
X2117800284Y-2055844969D01*
X2075762772Y2137569364D01*

The line width is 2.54mm so it looks like some inch/mm conversion went wrong.


#10

@bobc - thank you so much. I have implemented this and it works as expected.

No idea what caused it though? How did you spot in within the gcode? You must have some special goggles :sunglasses:


#11

I just deleted each block until the lines went away…although I should probably have guessed a line with of 2.54mm is unlikely.

I’m still wondering where the lines come from, but knowing the width they should be easy to search for.


#12

as pointed out by @bobc and @Rene_Poschl it could also be gr_text (unlikely if the source was DXF though?).

Check for something with the end of the line having the width field that Bob mentions.


#13

I will investigate tomorrow … I have a very long train journey :slight_smile:

Thank you all for such rapid and helpful responses. I really do appreciate it…