How to correctly create PCB screw terminal PCB footprint?

[matrixofdynamism]

I intend to create PCB footprint for a basic part. The datasheet for this part DG350-3.5-02P-14-00A(H) can be found at https://datasheet.lcsc.com/lcsc/2106062140_DEGSON-DG350-3-5-02P-14-00A-H_C2760668.pdf.

I am using its 2 pin version of this part. In order to make the foot print, I am not sure how large to make the through-hole via pad and hole size. More specifically, it is not clear what to enter into the dialog box that we get from Footprint Wizard. I have attached a picture of it to this post.

The footprint wizard has one textbox for the hole size. But why are there so many for the pad size? I have made red box around the textboxes.

[T3sl4co1l]

See: https://www.altium.com/documentation/altium-designer/pads-vias#!pad_properties particularly the top-middle-bottom pad stack scheme.

Most likely a simple pad (same size on all layers) will do, i.e. enter equal numbers here.

Is it really worth using a footprint wizard?  You don't even get the correct 3D model out of it, and it's just 14 objects, at least as I'd draw it.  Well maybe more, I do like me some silkscreen artwork, but for the basics including outline and courtyard info, yeah.

Tim

[floobydust]

The datasheet shows a recommended footprint of a 1mm hole size on the 0.8mm dia pins, which matches what I have for IPC Level C. Hole around 20% bigger as a minimum.
Pad size around 2x the hole size is pretty large (annular ring), for through-hole parts that need grip and see a lot of torque like a terminal block.
I use that when possible and IF there are no high-voltage spacings required between the pads. The pins are 3.5mm apart, that would give 1.5mm clearance.

Altium shows the pad stack that I think allows you to specify inner layers smaller pad OD for the annual ring spec you want.

Those terminal blocks I find cheap as the spring stays stuck down once you remove a wire, so I kind of hate them.
The sliding cage clamp ones are superior but could not easily find at LSCS, that website is primitive.

[matrixofdynamism]

I made first PCB last year using Altium, my employer has Altium license but this was done by me to learn the software in off time. But then due to work pressure I had to stop doing the learning. I am trying to pick up from where I left off and this time I want to continue until I achieve satifactory progress.

What does IPC really say about the sizing of hole and pad taking into consideration that there is tolerance in the pin size and there is also tolerance on the drill that shall make the hole? Also, taking into consideration the fact that there must be sufficient area for solder to bind the pin to the PCB that can withstand some shear stress which shall be created on the screw terminal during normal use.

In this case I am dealing with a screw terminal. However, it could be a connector used to connect PCBs together, or it could be an IC. How does one know how large to make the hole and pad in reference to the pin? I would assume something like (just random) hole 25% larger than pin and pad twice diameter of the hole. I don't know how professionals do it though.

[ajb]

Getting away from Altium-specific discussion here, so you might get better discussion on another subforum. 

There are lots of resources out there that discuss IPC requirements, and you can even find copies of many of the standards documents floating around on the internet. 

As far as accounting for manufacturing tolerances in your footprint design, in general you first have to determine your limiting values--for example, the minimum pad size that will result in an acceptable solder joint, and the maximum pad size that will allow for adequate clearance from adjacent pads/tracks.  Let's say that's a minimum of 0.8mm and a maximum of 1.1mm.  Then you look at your manufacturing tolerances, which specify the range of actual dimensions you might end up with for a given specified dimension.  Let's say the tolerance on the pad size is +0.03/-0.05mm. That means a pad you specify as 1mm may end up being anywhere from 0.95mm to 1.03mm.  You can then subtract the positive tolerance from the maximum allowable pad size and the negative tolerance from the minimum pad size to determine what pad size you can specify.  In this example, that's 0.8 - (-0.05) = 0.85mm Min and 1.1-(0.3) = 1.07mm Max, so you can draw the pad at anywhere from 0.85 to 1.07mm and still be assured that the pad will be fabricated at an acceptable size.  That's an oversimplified example, but provides the basic idea.  Geometric Dimensioning and Tolerancing is a whole subject unto itself, and combining multiple tolerances (for example, in SMT parts you'd need to account for tolerances in the fabrication of the board, the component geometry, and in the placement of the part on the board) makes things more complicated.

That said, what are you really trying to achieve?  You can go very deep into the engineering behind footprint design, but that's just one piece of designing a PCB.  Getting into that after making your first PCB is kind of like going for a PhD in semiconductor physics after blinking an LED with a transistor.   You don't need to go that far to get serviceable results, especially for personal/educational/on-off projects.  If you're still in the early stages of learning PCB design, it's far better to develop a broad understanding of the whole field first.  Get a board designed, built, and tested, then get a second one designed a little better built and tested, then a third a little better still, etc.  Get a bit deeper in different areas each time, and make a note of what aspects of your designs worked well and what didn't. 

[nctnico]

For terminal blocks I prefer to use large, oblong shaped pads that offer some mechanical stability and heat dissipation. For pad size I basically go as large as creepage limits permit.

Be sure to derate the current by 50% in order to keep the temperature of the screw terminal within operational limits. I second the suggestion to go for cage clamp terminals (like the ones that Wurth sell). Even better is to use pluggable terminal blocks so a board can be swapped quickly. I have been using these for 10+ years and my customers are happy with then.

Personally I find it handy to mark the silkscreen with the direction in which a plug or wires are inserted. It is easy to place screw and pluggable terminals the wrong way around if the sides with the wire / plug entry isn't clear from the silkscreen.

[matrixofdynamism]

@ajb, the objective at this time is to learn proper techniques.

The PCB itself is secondary, it does not do any specific function.

[nctnico]

If the assembly is done in house, also make sure to talk to the people dealing with preparing the files. Maybe they can tell you how to make their workflow more efficient. If not then don't do anything special. For example: paste mask is specific to the production process. For that reason I always have the paste mask size equal to the pad size. Let the assembler tweak the paste mask to match their process & preferences. In my experience they all have their own, unique combination of oven & paste. I have had a situation where an assembler couldn't deal with a QFN for which the space between the pads was less than 0.2mm (using the manufacturer recommended footprint). They had solder briding issues on every boad. OTOH another assembler didn't have any problem with the design. The latter likely tweaked the layout a little bit or used different solder paste.

[Alti]

The datasheet for this part

That is a terrible screw terminal design.
Get a proper one. You do not have to buy Wurth or Amphenol but for reference it is useful to have one original (for reference) de-soldered from some scrap. Buy clones of good designs.
But if none of the reputable companies makes such junk - I would not go that path.

One more remark - from my experience, if some gear fails, 30% are a result of poor wiring/terminals/connections. Due to corrosion, abuse, cracked solder joints or juniors creating PCB footprints for screw terminals.

[matrixofdynamism]

For now I am just designing PCB to learn the process properly. I have concluded that it is a good idea to get similar part footprints from snapeda and have a look at them for guidance. What do you think?