After some hesitation I decide myself to ask for your expertise. Sorry if I should be able to find the answer somewhere else but I spend a couple of time searching for it without any success.
We are a very small team part of a startup and working on some electronic products.
Our electronician uses KICad to develop PCBA.
We are going now for manufacturing but our EMS is asking for the ‘‘Components Implementation sketch’’ to be able to go through cabling the PCBs and…our engineer does not manage to release a proper one.
Is that part of accessible function with KICad ?
Any help or information would be welcome :
Below you will find an example of what our EMS is asking for. We do manage to get something but most of the components are not readable especially in the areas where they are a lot of them.
Thanks by advance to those who could help us in that.
What we can get : OK in area with low component density but as you can see when we have a lot of them we can not manage to read that much : (soory as a new user I can only get on image)
The best way i konw of is to have the reference designators of your parts and an outline on the fab layer.
You can add a second reference designator to your footprints by adding a text field with text %R.
(My symbols have the main reference on the fab layer and a second designator on the silk layer.)
If you do that with all your footprints you can just print the fab layer and you get what you want.
If you don’t want to do that maybe the silk layer could also work. (depends on how you designed your footprints.)
That is essentially the method I use. See atch for examples.
I use the “ECO1.User” layer for the assembly sketch, rather than one of the “Fab” layers. The main reference designator goes on the top silkscreen, as well as the main value - almost always set to “Invisible”. I use the %R and %V notation to put the information on Fab and ECO1.User layers.
Note that you don’t have to follow any of the “rules” for silkscreen when you create the assembly sketches (on whatever layer you use choose). Fonts may be larger or smaller than what you use for silkscreen. Lettering may be placed on the component bodies, or over what is normally bare copper. If you are artistic, the components can be represented by detailed representations of their physical appearance. You may also add special instructions, hints, or warnings to this layer.
@all, is that kind of ‘job’ also solvable with those assembly drawing scripts that some users have produced, or do I mix stuff up here?
Esp for SMD components it can get tricky to get all that information on a single sheet of paper.
The reason why i have the main reference on fab (in your case it would be eco) layer is because than i can set all of them to visible / invisible in the render tap.
(got this idea from a post by @Joan_Sparky)
During the layout process i only show the fab layer (with values hidden via the render dialog), the crtyd and the copper layers. I also have the references inside of the components in a small font so that they do not hinder me while i route out my board.
I do include component references on an auxiliary layer (Comments in my case). When plotting gerbers I enable the “Plot footprint references” checkbox.
Then in GERBV (I used GEDA’s GERBV for gerber proofing) I include layers I want to have in an assembly drawing (outlines, drawings, comments etc.) and export PDF from there.
Works for me.
We tried doing the different way you all have been suggesting, more or less successfully, as now we face another kind of issue :
On the PCBA we have some ‘‘high density area’’ with a lot of components.
If we keep the silk on the PCB and want to generate implementation of component drawing than it become unreadable. As you can see on the drawing below :
I for one am against removing the silkscreen.
(but i don’t think it is a requirement for anything. But it might depend on the agreements with your customer)
My reasoning is that it is easier to fix a pcb when you have references.
What we wanted to show is that one can have two separate references. one for the documentation and one for the silkscreen.
(you might even have 3. one very small reference for use during routing.)
@Rene_Poschl : Thanks, If I understand correct you say that we can also have two kind of documents : One with the silkscreen (only) and one with components identification (only) ?
In that way the implementation of components document would be readable but is it still useful if you have only the components without their location ?
I mean you should then use both of the documents to locate properly the components once the PCB has been assembled ?
Or maybe print the Component implementation sketch on some transparent paper ? I feel like I heard of this somewhere…
(My answer takes my above mentioned standard as an example)
Yes. You build your gerbers as you did until now. (These will contain the copper layers, silkscreen, edgecuts and so on.)
And maybe even the fab layers if they are used by your manufacturer. (ask them how they want the documentation.)
Additionally for documentation you can print whatever layer to pdf. (Use the print dialog not the plot dialog!)
To get something similar as you mentioned select the following in this dialog:
Select the technical layers you want (edge cuts + fab)
maybe select copper layers (then you need to print in color. The colors are taken from your rendering settings)
also remember things that are invisible (ore hidden in the render tap) are not printed.
What about different text sizes? where should this information go?
What if you want the text on the silks layer outside of the part but the fab reference inside of it, …
Yes maybe making footprints could be a bit faster with something like that but i think the current system allows more flexibility.
Good points! I originally considered this idea when dealing with text other than the reference. But you’re right, you may want it to appear differently on each layer.
