FEDEVEL
Platform forum

mulfycrowh , 02-20-2022, 02:23 PM

Hi everyone !

There are components like the one attached where it is difficult to apply this rule.
I guess it would be convenient to deactivate the rule for such footprint.
I see that in the Query Commands we have one command Footprint which returns all components matching the given footprint.

What would be the syntax ?
There are First and Second objects ?

Thanks a lot.

Lakshamana Balakrishnan , 02-21-2022, 02:46 AM

HI @mulfycrowh , If you need to control the soldermask you better apply "solderexpansion" rule to that either component or component class to waive out the minimum soldermask silver. If you waive out minimumsoldermasksilver rule directly, Manufacturer will not accept less than 3mil-5mil Solderweb.

mulfycrowh , 02-21-2022, 04:41 AM

I was asking about the way to delete the rule for one component

robertferanec , 02-21-2022, 05:50 AM

@mulfycrowh, normally, when creating this footprint, I would make solder mask opening smaller to achieve the sliver width between the pads at least 0.1mm (often 0.065mm still can be manufactured) and I would adjust the rule globally. If your PCB manufacturer can't manufacture it, they will remove the solder mask between the pads - you can do that too - just draw a rectangle around the pads on the solder mask layer, but this may increase possibility to have short circuits between the pads.

PS: Rules are there to be sure your PCB manufacturer can manufacture the PCB, so the rules should be set based on the capabilities of your PCB manufacturer and if needed, then the problems should be fixed rather than waved. Waving may not help with the real production.

mulfycrowh , 02-21-2022, 01:29 PM

For some components like the one attached, it gives a very small solder mask if we want to have a 0.1 mm solder mask opening.

mulfycrowh , 02-22-2022, 01:20 PM

@robertferanec Robert, I would like to know what you think about this footprint.
Space between pins is 0.5 mm.
I applied a solder mask of 0.075 mm in order to get a solder mask opening of 0.1 mm.
The problem is with the central pin MH1.
We have no space to get a solder mask opening of 0.1 mm.
Can I keep it like the attached screenshot ?

qdrives , 02-23-2022, 02:10 PM

Does MH1 need to be plated? This may also give electrical clearance issues.
And name the mounting holes different MH1, MH2, etc. as both are now called MH1.

mulfycrowh , 02-23-2022, 02:27 PM

They need to be plated.
Attached picture and drawing.

robertferanec , 02-24-2022, 05:28 AM

That is an interesting connector. I would probably connect the closest pins to the hole and also the hole to the same net (e.g ground) - that would solve the problem with soldermask and also you would be sure if there is a short circuit, nothing would happen. The space between the hole and closest pins looks super tiny.

WhoKnewKnows , 02-24-2022, 05:36 AM

I find that when I view the footprint in the library view and the solder mask is set to follow rules instead of manually set, the rule it follows while viewing in the library has a much larger expansion setting than the rule setting in the PCB project I'm working on.

To get a realistic sense of the actual appearance, I either have to set the expansion manually temporarily while viewing in the library, or temporarily place the footprint in the PCB in the current project.

WhoKnewKnows , 02-24-2022, 05:39 AM

What does the connector manufacturer recommend for footprint specs?

qdrives , 02-25-2022, 02:54 PM

Datasheet states 1.0mm slot. There should be 1.5mm between the pins. 2x0.15mm anular ring (tiny) leaves you a spacing of 0.2mm. Oh, but the pins are 0.25mm, so it is not possible.
Why is the slot drawn horizontal? That way, you just as well use a round hole. I assume vertically you do not need the space?
This seems again a connector where the manufacturer did not think about fabrication. USB C connectors are similar.
I would measure the width of the pin (it is not in the datasheet) and either use a (round) hole or a vertical slot, ignoring the datasheet.