So I’m following this tutorial on YouTube(by Phil’s lab) and mid way through I came across this issue that there is a purple color around each component in the figure to the left(tutorial), but I don’t know how to get it on my PCB or does it even matter?
I’m new to kicad and PCB in general so don’t know whether I should move on with my layout so far.
It’s the mask opening in the F.Mask layer. It depends on the board manufacturer if they want you to set a larger mask opening than the pad, or if they want the opening to be identical to the pad and they adjust it themselves for their manufacturing tolerances.
When the mask layer is active in the Pad Properties, the value for this “Solder mask clearance”, i.e. the amount by which the mask opening is larger than the pad, can be set globally in Board Setup -> Solder Mask/Paste, for each footprint in Properties, and for each pad in Properties.
You don’t have to worry about that yet, only before you generate the gerber files to be sent to the manufacturer. If you want to know more about the mask layer, read How does solder mask layer work?.
1 Like
Ahh thanx.
Does that means I need to change the “Via” (3v3) for all the places I have placed since according to tutorial they must be placed just near the 3v3, but If add this mask opening then 3v3 vias would be placed above the mask opening?
… and apparently I have to add some text to emphasize my quote from eelik to get above the minimum 20 character limit enforced by the forum bots.
1 Like
I always set the Solder Mask clearance to 0(zero).
The Solder Mask layer can be a little bit confusing at first because it is a NEGATIVE layer; it shows were Solder Mask will NOT be applied.
To understand this layer, turn off the copper layers in PcbNew. Also, change the clearance to something much larger, and also a little negative, and check the results with the 3D Viewer.
Hint: You can change the color of the Solder Mask layer both in PcbNew and the 3D Viewer to be the same color.
1 Like
This is not a good idea.
Placement of the solder mask always has some tolerance during PCB manufacturing. This means that if you set this clearance to 0, the exposed pad area which is available for soldering will vary between batches. When all the planets (euhm, layers) line up, then the exposed pad area will be the same as in KiCad, but in all other instances the exposed area of the pads will be smaller.
@Sprig Have you looked at your PCB’s with a magnifying glass? You may well se a small sliver of exposed FR4 on one side of a pad, and the solder mask overlapping the pad on the other side of the pad. But it is indeed also possible (and I think even common) that PCB manufacturers modify mask expansion to accommodate their own manufacturing process.
It’s not their choice. It’s your choice.
With a simple search:
https://html.duckduckgo.com/html?q=mask+defined+pad
The first hit is from allpcb, and it has a pretty good explanation of the two variants.
https://www.allpcb.com/soldermask/pads.html
Note that you can not just switch willy nilly between those variants. KiCad’s libraries are designed with the assumption that the exposed pad area is defined by the copper.
If you want the exposed area defined by the solder mask, then the pads should be wider, and this would require a duplication of all of KiCad’s footprint libraries.
You may want to look at that youtube video again.
Apparently KiCad defaults to a solder mask clearance of 0, and it’s likely that they changed the solder mask settings earlier in the video.
Short Version:
IC manufactures are now making smaller parts with tighter tolerances than some PCB manufactures can’t keep up with. Setting the Solder Mask Clearance to 0(zero) informs the PCB manufacutre that Solder Mask between pins is a design request.
It’s “your choice” only in the sense that you can choose whether or not to use certain manufacturer with certain requirements.
But I’m not sure you have understood correctly. Some manufacturers want 0 clearance because they will adjust the clearance themselves. It’s also not as simple as just setting the clearance. For a large (panelized) board the adjustement may be relative, i.e. different in different areas of the board (source: some document from the Ucamco website).
Adjustement should not of course be applied to real solder mask defined pads. Even in the design phase there should be enough copper in those to allow registering errors (moving the hole mask layer in x and y directions). For copper defined pads the clearance is for this registering error, so that the mask never covers the pad partially.
I’m a bit apprehensive in making assumptions on how PCB manufacturers handle this. Even if there are “common practices”, then not all PCB manufactures will follow them. So to be sure you have check with your PCB manufacturer, (or at least their website) for how they handle this.
I also think that milad has been given much more info then he asked for. At least he knows now what the purple borders mean.
1 Like
KiCad may now have the Solder Mask default to 0(zero), but it did not in the past. There are a number of posts on this forum where members used the default value and had un-useable boards fabricated.
From earlier discussion, there just is not any good reason, in my opinion, to deviate from setting the KiCad Solder Mask value to 0(zero) for the average/normal design.
All of the boards that I have had fabbed by using OSHPark (not a sponsor) have been perfect with a KiCad setting of 0(zero).
I see nothing wrong with a KiCad specification of 0(zero) and getting a small deviation due to tolerances during manufacturing.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.