Hi. I finished my pcb artwork and opened the bot layer mask file, and I am writing because I have a question.
This is the file I opened. I think you can think of green. It’s usb c-type and it looks like all 12 pins are connected. I will also attach cu pad layer.
I have a question here. The reason all 12 pins are connected in the mask file is that all 12 pins are short? Or is the gerber file created properly?
It’s right that everyone should not have short!
I am not sure what I am looking at here.
My best guess is that Red in the gerber view is from a copper layer, and green is from the solder mask cutout.
You’re right. I just want you to think of green. If you look at the green, it looks like all 12 pins are connected.
I want to know if all 12 pins are short or good.
I was reading.
If the minimum distance between the masks is 0.15mm, then should I reduce the solder mask clearance by more than 0.051mm and adjust it to 0.15mm?
When pads are too close to each other it is normal practice to have one opening in solder mask for all of them. The key problem is how wide the thinnest solder mask bridge between pads can be. It depends on PCB manufacturer technology possibilities - they should have such info to be read.
You must check what is the minimum amount solder mask opening are bigger then pads and what is the minimum for that bridges. If it can’t be done then you should have one soldermask opening for all pads.
Too tiny solder mask bridge may tear and stick elsewhere.
My rule is: solder mask increase should be 3 mils and bridge should have 3 mils so if between pads there is less then 9 mils then make common solder mask opening.
The article is an interesting tutorial on solder mask indeed. However, it does not discuss why we apply add a clearance to the solder mask at all.
The purpose of the solder mask is to protect the board and assist in the assembly process. The ideal solder mask is one without clearance, where the solder mask opening matches the pad exactly. This is what the designer ideally would want. The problem is that the fabricator cannot deliver this: there are unavoidable deviations in the fabrication process. The cost of the deviation is very assymetric: mask on the pad is a disaster, a clearance around the pad is no big deal. Hence the need for a clearance. Another issue is the minimal width. Appyling a larger clearance aggravates the minimum width problem. The ring to be as small as possible, but no smaller.
The question is how much clearance to apply. This is very complicated: it depend on the equipment, the process, the mask type, the copper weight, even the mask color. The capabilities published by a fabricator are a crude simplification of a complex reality. The designer may not even know where the board will be fabricated. In short, the designer cannot know what the ideal clearance is. Whatever clearance he applies, the only thing he knows for sure is that it is not be the optimal one. The only person that knows the ideal clearance is the fabricator, at the moment of fabrication.
The fabricators have a CAM system and are quite capable to optimize a mask. Complicated stuff must be done to get to the required via protection. As quite a few masks are wrong, they are used to remove the applied compensations, and re-apply them to their requirement. This is one of the things CAM engineers do to make a living.
Hence, the best clearance to apply is no clearance at all. Let the fabricator apply the clearance that best suits his process. If you want to have minimal problems, send the fabricator the mask without extra clearance, and let him compensate for the deviations in his process. After all, he applies other changes to compensate for deviations in fabrication: copper is spread to compensate for over-etching, and layers are scaled to compensate for distortions in the lamination press. We do no not expect the designer to compensate for these, do we? If we don’t to it for etching and lamination, why do it for the solder mask?
Many manufacturers seem to give a value which you should use, and they don’t tell they would do it themselves. It’s of course possible that if it’s set to zero they do that. But if you want to be sure you have to ask (as is the situation for most other things, too).
I didn’t of course mean that they wouldn’t compensate for the mask registration error. I meant that whose responsibility it is to set the clearance is an opinion, not a fact. I’m not going to quote anyone because whoever uses a manufacturer must read their instructions anyways, and they differ. I once skimmed though a dozen or so just to compare their capabilities and information and noticed that some want it to be zero in the design and some recommend some value.
Zero clearance goal is not that good of an option. This is because if you really get 0 clearance then you increase the risk of delamination. So you should always aim for slightly larger or slightly smaller than 0. (Soldermask defined or non solder mask defined)
Also every fab worth their money publishes detailed requirements (possibly even detailed tolerances such that you can go closer to the “edge”). So i really don’t understand why you would let them do your job. Reason being that if you let them decide on mask cutout then you will get what they think is best. And because they are not the designer means the work with limited information here.
To be honest everytime a fab thought they know better than me meant they needed to send me a second patch for free because well surprise surprise they did not know better after all. The good thing is that as i designed the board for their documented requirements means they were in breach of contract by changing my design (without prior notification) which means they were responsible to fix it. If you use 0 clearance and anything goes wrong they will point you to their requirements page and you will foot the bill here (you will have a hard time to argue otherwise).
I mean of course i never ordered at a pool processor that subcontracts out to some other manufacturer (most likely a different one each time). I always ordered directly at a manufacturer so the published requirements are the requirements of the process.
This does not mean that one can never do what you suggest. I would however hesitate to suggest it to anybody else as it can backfire quite badly. (Letting the board house decide might be a good option for small scale production or if you hand solder anyway. Definitely not if you are at all concerned about yield or longevity of your product)
Indeed!
Maybe there is no single right answer. I suppose that if you work at Samsung on high volume products, in a vertically integrated environment where the capabilities are very well defined, you pretty much create the solder mask as you are told. But does this apply for say a machine controller, fabricated in the open market, for modest volumes?
The capabilities of a fabricator are complex, depending on sizes, thicknesses and even color. (It even changes of time, many capabilities are not hard limits, but are driven by yield considerations. A fabricator that is hungry will accept lower yields, and thus tighter clearances.) There is the matter of competitive confidentiality. These are the reasons that efforts by CAD to have fabricators specify their specs in detail have failed. Rene_Poschl is concerned that if you deliver the mask 1:1 you will be defenseless if he screws up because you have not defined what he must make. But there are so many other aspects of a mask where he can screw up, mask thickness and so on. You must either have some confidence in your fabricator, or refer to a spec such as IPC-6021, that describes mask in detail, including in how far they can encroach on lands. Sending the design with a mask clearance is really of no help. In fact, I think IPC recommends supplying the mask 1:1, but I admittedly do not remember where. So I stand by my opinion that most, if not all, fabricators are able and willing to handle the mask clearance in CAM, and that will result in the best choice of clearance, and hence the best quality.
@Rene_Poschl, you had a bad experience with a fabricator messing up your design. Can you share the details? Others can learn from your experience.
