F paste for SMD

I am using a quectel module. I checked different forums that the F paste should be smaller than the copper pad,so I edited the paste and made it smaller. I am wondering which among the both would be suitable.
The footprint given:


After I edited:

Forums? How about the datasheet? Please give a link to the datasheet or some other information by the component manufacturer.

I checked different forums that the F paste should be smaller than the copper pad …

this is a general rule of thumb and not that bad if you have no other sources. But as @Ax111 said: the best advice should be the datasheet.
But even that is not a law: the recommended pad/paste dimensions depend also on pcb-manufacturer/stencil-thickness and much more - so it’s not forbidden to differ from the official recommendation.

Since ‘always’ (30+ years) I used F paste exactly equal (thermal pads with vias are the exception) to pad and no one told me that it should be smaller. Contract manufacturers (we used 2) who from my single PCB make their panels (size according to their needs) are used to do all needed modifications without asking unnecessary questions. It is because they are who then use paste stencil and not me.

The reason for paste being smaller than copper is that copper has its thickness (the pads are higher than the PCB around). The small (negative) margin around each pad is to make paste opening fits tightly to the copper pad even when stencil positioning is not accurate. If it not fits tightly then during applying paste it seeps under the stencil at the pad edges, soiling it from the bottom. Then the stencil has to be cleaned before next use what is not what they want to do.
I know that my contract manufacturer lefts 1 mils margin, but it can depend on achieved accuracy of stencil positioning. When he had a problem with pads with rounded corners (I have never used such before KiCad and he had no tool to modify them) we agreed that I have set in PCB Editor Board setup - Solder Mask/Paste - Solder paste absolute clearance to -0.025mm and paste gerber generated meets his requirements.
You need not to do it by defining separate pads at paste layer in your footprints (thermal pads are exception).

Best I know, there is no unambiguous and clear answer to this quiestion. For example, solder stencils can be ordered in different thicknesses , and this greatly influences the amount of solder deposited on a pad.

Making the F.Paste cutouts lager then the pads themselves is a valid approach, and used in some cases to increase the amount of solder deposited on a pad. During reflow, the pad will wick it up. But Piotr also has a valid point. solder paste can get under the stencil more easily when the stencil openings are bigger then the pads.

In the end, I should not worry too much. For small production runs, a bit of rework is acceptable, while for big runs, solder stencils are cheap, and they can be tweaked to improve yield and lower the amount of rework.

I am not familiar with those quectel modules. Do you have any info on who made that first footprint?
Both variants probably work, but there is one general thing I do not like about your edit. Round corners for the solder paste stencil are good. First, very sharp corners are dificult to make, and each manufacturer will have some unspecified minimum corner radius. (so you will get different stencils from different manufacturers). Second, solder paste has a tendency to stick more in corners, and this will also introduce a variation in the amount of solder paste on the pads. Solder paste releases easier from round corners.

So did I. Paste is same size as the pad. The stencil manufacturer reduces the openings by 5% and I never had a problem with it.

hello, thank you. I have downloaded the footprint from the ECAD website only. I would definitely make the corners round as you said.

I would go for it then.

hey, i have attached the reference below

The clearance is really small as the pad thickness itself is less. So I should then leave it to as it was?