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