Use module as board outline

[lawrencek]

Is it possible to create a module and place its drawings on the board outline layer? The layers that look as if they might work are the FAB Top and FAB Bottom (I think that is the name - one has the same colour and is the last in the list).

If I can do this, then I can have a set of outlines that are fixed and can be accurately defined - would be great.

Lawrence

[bobc]

Yes, I have used this method to create board outlines for PCBs which have a specific shape, and are not a simple rectangle. For example, PCB for Hammond 1553 box, Arduino. I also found using arcs in the board outline very buggy in pcbnew, so generating them externally allowed precise control.

I’m not sure what the FAB Top and Bottom layers are, those are new for me. The layer I used is “Edge.Cuts”. I also placed NPTH holes for mounting holes. There are some restrictions on the layers that can be used in a module. e.g. only text on front side.

I haven’t yet tried with Kicad v4, but the principle is hopefully the same.

[Joan_Sparky]

@lawrencek

Is it possible to create a module and place its drawings on the board outline layer? The layers that look as if they might work are the FAB Top and FAB Bottom (I think that is the name - one has the same colour and is the last in the list).

If I can do this, then I can have a set of outlines that are fixed and can be accurately defined - would be great.

Yes it’s possible, but it has drawbacks
How:

• draw the outline on F.Silk (should be default when you start drawing in the module editor).
• then open the module in a text editor and change the layer from F.silk to Edge.Cuts.
• don’t open + modify + safe this module in the footprint editor again or you have to repeat step 2, as the editor will move anything that’s on Edge.Cuts to F.Silk/etc…

IMHO I’d advise against it though as KiCAD doesn’t really like it.
I draw the outline for footprints on the Dwgs.User and for cutouts on Cmts.User in 0.05 thickness and redraw them in pcbnew.
Don’t find the arc drawing buggy, as I usually use just 90deg for this method and stay with 0.25 or 0.5 mm grid.

See this thread/post of me (explaining the edge.cuts in footprint editor)… also another example further down of how I’d do the outline for a RPi-Zero-Hat:

Raspberry Pi B+ Hat Template

As you can see up there with Aquila it’s confusing and not straight forward for noobs Hm… have you had a chance to look at the footprint I attached up there for a 100x100 board? I find it very easy to follow the outline on the drawings layer with segments/arcs on the edge cut layer. This then also can be pulled in an existing project where much of the layout has been done already (for conversions for example)… and messing up the mounting holes/cutouts is pretty hard that way also, as …

And yeah… Cmts.User color and Dwgs.User color deviate from the standard KiCAD setting… like it better that way and nicer to my eye

[lawrencek]

I created a testpcb module and edited the module file with a text editor. It worked and I could print the edges. But when I saved the PCB and opened it, it crashes.

It seems as if only a small change to KICAD to allow edges in the module editor, and then PCBNew to all them there.

I could possibly make a post processor to do the changes so that it makes the correct output file.

I could make a board outline using a standard module, and the edge on the front silk or a legal layer and simply use it as a template to check the layout and trace the edges over it.

I have seen “templates” discussed, but it seems as if these are standard PCB designs and you then append them. But it would be nice to group the items.

It would be useful to have this as a standard feature of PCBNew

Lawrence

[Joan_Sparky]

@lawrencek

It seems as if only a small change to KICAD to allow edges in the module editor, and then PCBNew to all them there.

That’s a philosophical thing afaik - the devs don’t want to be able to do this in the fp editor for footprints…
Might even be defined as ‘bad practice’ in some standard for ECAD software somewhere… who knows.
At least one can change the layer for drawings to Cmts.User or Dwgs.User.

@lawrencek

But when I saved the PCB and opened it, it crashes.

Which version was that?
Can’t remembering that happening in mine BZR6097…

[s_light]

i have done the thing with

• drawign a ‘footrpint’ with my board outline on F.silk
• open in texteditor and replace F.silk with Edge.Cuts.

and all went fine.
the only thing that is sometimes a little annoying is that the footprint is ‘everywhere’ when you click inside the pcb…
for this a option for ‘footprint only selectable on edge or line’ would be great…

sunny greetings
stefan

Application: kicad
Version: 0.201512080931+6353~38~ubuntu15.10.1-stable release build
wxWidgets: Version 3.0.2 (debug,wchar_t,compiler with C++ ABI 1009,GCC 5.2.1,wx containers,compatible with 2.8)
Platform: Linux 4.2.0-19-generic x86_64, 64 bit, Little endian, wxGTK
Boost version: 1.58.0

[lawrencek]

I have gotit to go now with the latest KiCAD 4.0.1. and it did not crash.

It would be a simple change to allow KiCAD module editor to have drawings on the Edge.Cuts layer, with perhaps a warning if needed. I can write my own utility to do the changes from a known layer to edge cuts. but the fact that I can accurately define the the card layout is great, and of course I can now have predefined pads, labels etc all in one place.

Can you take out the restriction for the layer selection?

Thanks

Lawrence

[PCB_Wiz]

I’ve bumped into this issue with Translators…

This is what I find - (June 19th Build)

@Joan_Sparky

Yes it’s possible, but it has drawbacksHow:- draw the outline on F.Silk (should be default when you start drawing in the module editor).- then open the module in a text editor and change the layer from F.silk to Edge.Cuts.- don’t open + modify + safe this module in the footprint editor again or you have to repeat step 2, as the editor will move anything that’s on Edge.Cuts to F.Silk/etc…

IMHO I’d advise against it though as KiCAD doesn’t really like it.

KiCad can import & save Edge.Cuts ok, in Kicad_Pcb files.
KiCad can also Save to Library, via footprint editor (do not edit any lines! (as above))

@Joan_Sparky

It seems as if only a small change to KICAD to allow edges in the module editor, and then PCBNew to all them there.

That’s a philosophical thing afaik - the devs don’t want to be able to do this in the fp editor for footprints…

Why not ? Software should not limit the user control over the data. To me, that is a simple bug/defect.

Fills seem to work just fine with a Footprint based PCB outline.
Data imports and saves to library also ok.
It is only the Footprint Editor itself that is out of step here.

Maybe the issue they were avoiding by limiting the Editor, has since gone away ?

@s_light

and all went fine.the only thing that is sometimes a little annoying is that the footprint is ‘everywhere’ when you click inside the pcb… for this a option for ‘footprint only selectable on edge or line’ would be great…

I find pick-footprint is by nearest ( I think it uses the bounding-box of PAD-Edges, plus outlines, if any) - you have to be well clear of a real footprint (outside that bounding box), to catch the board outline, so in practice this issue is there, but can be avoided.

[Joan_Sparky]

@PCB_Wiz

Why not ? Software should not limit the user control over the data. To me, that is a simple bug/defect.

Fills seem to work just fine with a Footprint based PCB outline.Data imports and saves to library also ok.It is only the Footprint Editor itself that is out of step here.

Maybe the issue they were avoiding by limiting the Editor, has since gone away ?

You have to take that one up with the Devs on the mailing list… I’m just an enthusiastic forum moderator who uses KiCAD on a frequent basis

My personal opinion… it should be possible, yeah, but I can definitely life with it as-is and for sure would find other stuff more important and Dev-attention worthy than this.