Silk Off The Board, Wont The Fab House Screw Up?

[Mechatrommer]

picture showing part of the pcb i'm working on. since i want a component (trimpot indicated by semicircle silk on top) protruding out off the board, resulting its silk too. gerber export previewing it doesnt get cropped. so i'm wondering:

1) is there any way we can manually cropped this silk in DipTrace?
2) if i send this gerber silk to pcb fabrication house, wont they screw up the position of the whole silkscreen? i'm afraid they will try to fit the whole silk on the pcb resulting misalignment?

noob questions... i never send anything to fab house before.

[deephaven]

I've had this a few times and never had a problem with the PCB manufacturer. They are usually switched on and know what you're trying to achieve. Of course YMMV. Alternatively, can't you edit the shape so that it is a special for your board? Not familiar with your layout package so I don't know if that's a difficult thing to do for you.

[Mechatrommer]

Alternatively, can't you edit the shape so that it is a special for your board?

yea should be possible, only specific for this board. i keep thinking its a cheating method edit: but if fab house doesnt have any problem, maybe i can just send them this and let the excess silk go down to their machine's floor while printing. i dont mind, as long as the other silks are printed correctly.

[ToBeFrank]

I've also never had a problem when doing this.

[Time]

lol They wouldnt just move your whole layer and screw it all up in order to fit that on. you're good.

[mikeselectricstuff]

If you're ordering multiple boards it's possible it may spill onto an adjacent panel, however I'd expect that the most likely action is they'd just crop it.

[Mechatrommer]

so that means in the gerber file, there is coordinate system and info common to all layers? (pcb, silk, mask etc layer) maybe they use that coordinate info as-as regardless if the silk spill out or not? isnt it? i dont know gerber format, so i'm assuming there is coordinate system.

[thilo]

Why don't you ask them?

[Alex]

You could modify the footprint?

Anyway, this will most likely be picked up when they verify the gerber files and anything outside the 'dimensions' layer will be cropped. The last thing they will do is move the copper. That would generate so much publicity for them...

[Jon Chandler]

The only time I've had a problem with this is when I've created a panelized board myself - laid out a panel with a number of boards of the same or different design,  In this case, overhanging silk screens end up on neighboring boards.  Where the fab house has put together a panel, it's never been a problem.

What I like to do is put the overhanging part in a layer that doesn't show on a silkscreen.  In Eagle, the document, tdocument and bdocument layers don't go into the silk layers on the Gerber files, so putting the overhanging parts in one of these layers works well.  For example, with a right-angle BNC connector, the threaded part and barrel on on the document layer.  You can tell the proper placement at the edge of the board, but there's no worry about the overhanging part as it won't be in the silk layer.  In the picture below, the black lines are in the normal silk layr (tplace) and the magenta is in the tdocument layer.

[Mechatrommer]

i can turn off the marking (text) but not the silk (semicircle shape) in diptrace. i'll check again if there's any layers trick there. if it spills out to neighbooring board, it will be problem if it hits on top of smd mask, if there's any. but i think my board is ok since all of them through hole on that side. so soldering will be on another side. i will make the "my selected fab house later" famous if they spill the silk to another board, they should crop it, yea! they should.

[Dr_Ram]

i can turn off the marking (text) but not the silk (semicircle shape) in diptrace.

Here is something else you can try: use gerbv, the well-known gEDA gerber viewer. What makes it special is that it's one of the few free viewers that actually allows you to delete pieces you do not want and reexport in RS-274X format (it does very clean RS-274X exports). I have used gerbv to fix precisely this sort of problem for many folks who sent me their PCBs with bits of knob etc. sticking out in their silk.
Why not leave it to the fab house to do this? The board houses normally do crop anything outside the board outline but they can mess it up if silk overflows into an adjacent board on a panel, especially in a multi-design panel.

[48X24X48X]

They will crop anything outside of the board outline.

[Mechatrommer]

Here is something else you can try: use gerbv, the well-known gEDA gerber viewer. What makes it special is that it's one of the few free viewers that actually allows you to delete pieces you do not want and reexport in RS-274X format (it does very clean RS-274X exports). I have used gerbv to fix precisely this sort of problem for many folks who sent me their PCBs with bits of knob etc. sticking out in their silk.

thumb up! i thought i can do more detailed cropping, ie cut only some part of the object. but i lose the whole semicircle, its ok at least another alternative. thanks for your suggestion. btw the linux and windows version are separated, i only download for windows its version 2.5.0:

linux: http://gerbv.gpleda.org/index.html
windows: http://sourceforge.net/projects/gerbv/files/

Why do this? The board houses normally do crop anything outside the board outline but they can mess it up if silk overflows into an adjacent board on a panel, especially in a multi-design panel.

because in the post i stated i'm afraid the fab will screw up, but since most people say it will be cropped, then i'll just leave it hanging there.

[ivan747]

If you're ordering multiple boards it's possible it may spill onto an adjacent panel, however I'd expect that the most likely action is they'd just crop it.

What if you send a dimension layer to them. That would indicate the board ends at XY point and all the remaining silkscreen should be cropped because the chunk of board where the remaining silkscreen is either goes to the bin as excess material or it extends to the adjacent board, something nobody wants to let happen.

[thilo]

Amazing what you people do in order to avoid a simple mail to the manufacturer.

[jahonen]

Professional PCBs will usually include per layer title box describing the PCB and layer etc. in each and every layer so PCB manufacturer standard procedure must be to trim all things that extend beyond the board outline. That includes the silk too. Most CAM software have a straightforward function to trim the silk layer or other features. So don't worry about it.

Regards,
Janne

[shadewind]

I always do this for connectors and such things. Never had a problem. The board house needs to be pretty stupid to not understand what to do.