How to connect SMD pads internally

[Anonymous]

Hi 

I've created a custom SMD pads with a milling slot on both sides (named top pad as 1 and bottom pad as 1b) connected together in the library. But while routing it seems like they are not connected internally I have to route them separately. How to connect the bottom pad and top pad? Is there any other way I can do. I have added the screenshots below. Could you please help me.

Thanks in advance

[Anonymous]

When you create an SMD pad in the top and bottom layer they are two unique pads and are not connected. When you say they are "connected together in the library" in what way did you connect them?

It sounds like you want to create a slot shaped via or through hole pad but I don't know if this is possible. Maybe someone else might know, but what you may need to do is create one or more vias to connect the top and bottom layers. You may want to consider doing it outside of the pad area so it doesn't suck in solder.

[hudriwudri]

Use a through-hole pad instead of 2 smds. The hole will be milled out anyway.

And be aware that the corners of the milling rectangle will be rounded (minimum milling tool radius should be in the board house specs), so I prefer to draw it rounded with the correct radius to make sure the slot does not end up smaller than needed.

If you use this on a multi-layer board, don't forget to draw polygons on the inner layers as well, or you may get shorts at the milled slot.

[TravisJoe]

I will have to check again, but a via I believe will also force the "relation". I appears that just including them on the same net does not do enough in the application you are using. I have not done this with milling, but often do it a lot with thermal pads for higher power surface mount components. 

[Anonymous]

Hi 

Thanks for your suggestion. Below see my both attachments for top_side and bottom_side. This is the PCB already made. TP1 is the 12V line and TP2 is the GND. I forgot to put bottom pads while sending to the manufacturer and also I have wrongly made a whole board polygon with the name of GND at the bottom side. So bottom side TP1 and TP2 slot completely connected to the GND. So I've to cut the edges of the TP1 bottom pad to avoid connecting to ground and to make the board work. So I need to make a bottom pad like TP1 and separate that pad connecting to GND at the bottom side. Could you please provide any suggestion for this?   

[Anonymous]

Thanks for your suggestion. So, I need to put a via next to the tp1 to connect the top and bottom layer? The current I am using on the line is less than 100mA. Do you think putting a via next to the 12V line to connect the top and bottom pads is safe? Please see the latest board image I've attached at the previous reply. 

[Anonymous]

Is this for a connector or some very custom application? Typically a connector datasheet will tell you how to make the cutouts - often, a connector's pins would go through a round pad even when they are not round unless the expectation was to only utilize the solder side layer. Something to keep in mind - not sure if either work for your application.

As in my first suggestion, if you wanted to keep a non-round shape but maintain electrical (and thermal) continuity between top and bottom layers you can use vias to connect the top and bottom layers. There are a few factors to consider to make the right choice. It is a best practice to avoid putting a via into a solder pad because it can wick solder away from the component - so usually people put them in the copper plane of the pad but under soldermask. If your images the top and bottom pads do not look very big so you would have to decide to enlarge the pads to make space for this. Alternatively, rather than building it into the library you can use one or more vias on the board itself once you identify where you have board space.

Here is picture I found online of what I mean - in this case someone is using vias around a landing pad for a screw hole but the idea is the same for your slot. Picture is example only and I found it I did not make it.

 

Generally, 100mA is not very much current and one or more vias can certainly handle that for most applications. For virtually any current all you must do is determine the correct size and number of vias to handle your current load. I recommend Saturn PCB Toolkit (http://www.saturnpcb.com/pcb_toolkit.htm) to help you determine the best size for you. It depends on the copper weight of your board, the temperature environment you want, and any preference for either the size of the via(s) or the number. For example, because 100mA is so low, even a 10 mil via could handle the current but it might get too hot for your use case so then you could use 2 or more vias for added thermal reasons. Or change to a larger size via. 

My only suggestion would be to contact your board house to find out the copper weight of via plating - even if your board is "2oz copper" the plating inside the via may be less. For example, a board house I have used in the past will use 0.787 mil plating for vias by default even on a 2oz board, which is closer to only 1/2 oz and affects the ratings.

[Anonymous]

Thanks. it is for a custom application. So I can't change the pad size. As like the second image you've attached I can do the same for my application. Making a couple of vias next to the TP1 PAD and connecting the bottom layer to the top would be better. I am using 1oz copper. Do you think 20mil would suit? I will also refer saturnpcb tool.                                                                                                                                     

I am also having doubt in making a SMD_Pads. See below image I've named top as 1 and bottom as 1b. is that correct?

Top side pinBottom side pinMaking a package

[Anonymous · Accepted solution]

With regard to making the SMT what you have done should be ok. Although the Eagle convention would be to name them P$1 and P$2 by default you should be able to name them whatever you want - once you place the part in the schematic both pads will be renamed to the same net because you have them appended together in your device as both attached which looks perfect.  The only drawback is that you will have to place the connecting via(s) each time you use the component on a board and until you make the connection there will be an airwire between the top and bottom pads.

As for the via(s) size, you should refer to the Saturn PCB Toolkit to make your own determination because there are choices that will be unique to each designer such as whether the via is allowed to get 1 degree hotter than ambient, 10 degrees, 30 degrees, etc as well as depend on PCB thickness and plating. As I mentioned you should refer to your board house to get the exact plating for vias which may not be the same thickness as the copper used for the inner or outer layers.

That said, 20 mils via would almost certainly be fine for virtually any set of parameters for your low current needs. According to Saturn, a 20 mils via in a 62 mils thick PCB with 0.787 mils plating with standard FR-4 could handle more than 500mA with only a 1 degree C temperature rise. 

[Anonymous]

Thanks. Just wanted to make sure with you that I've done the right thing. Please see the routing image which is marked with yellow color.

Trace goes from SMD pad to the Diode both bottom and top using via's

[Anonymous]

It may not be the way I would have routed it, but the electrical connections appear to make the result you have described wanting.

Whether it is important to your application or not is for you to decide, but notice the current path between top and bottom SMD pads is a loop that travels through the vias as well as the diode's landing pad before getting back to the other SMD pad.

For many applications this will work fine, but there are some situations where this may be less than ideal such as high frequency or high noise applications. I believe you mentioned this may be a power input so high frequency is probably not an issue although I see the silkscreen mentions a pulsed input so then again it may factor in. If you plan to solder the component to both top and bottom landing pads then this should be of no issue because then the component itself will make a direct connection to both SMD pads through it's slotted pin. If you only plan to solder the component on the bottom side (which is typical) then note that any current drawn from the top SMD pad will have to come from the bottom SMD and travel through the vias and accross the diode's pad and trace back to the top SMD pad. If you plan to add more connections to the top SMD pad then it could be an issue.

A more ideal layout might be to place the two connection vias pretty close to the SMD pads so they can share the output load to connected devices. You could put them in line with the load trace or opposite to it. I made a quick example image showing two examples - I made the bottom SMD bigger to show clarity. I used a polygon to achieve the shape shown but a couple of wide traces would also work fine. If you have additional loads on other layers this may be more ideal - although again, what you had will likely work.

[Anonymous]

I got your point in making a loop. Also, the pulsed signal is less than 1khz. However, I want to make via(s) closer to the pads as like you mentioned. But my doubt is how would I connect the bottom trace using 2 via(s) on opposite side like the below image ? do I need polygon?

[Anonymous]

You cannot connect both top and bottom to your diode because it is only on the to side, but you can connect both top and bottom of your SMD pads to both vias. You could use a polygon on the top and a polygon on the bottom - but you absolutely do not need to. You could simply just use the route tool to create a trace from each via to the top SMD and then another two traces to connect each via to the bottom trace. 

[Anonymous]

Thanks. See the image below. I am not getting any complaint about the trace angles. I believe I have done the right thing now.