Doubts Creating Footprint for Duplexer QPQ1289

[qdrives]

The answers to your questions:

1a) No it is not necessary to add the bevel. It might help a bit for the assembler to properly orientate the component, but few designs will have it.
1b) If you work in Altium there are two possibilities to create the bevel:
- Use a solid region.
- In the latest version there is the possibility for custom pads. Like the footprint below, that also has a bevel in one of the pads.

2) Do not confuse the solder mask with the paste mask. The land pattern mask is for the solder mask. Perhaps they add it to make clear not to use Solder Mask Defined (SMD) pads. As it is all 50um, you can simply use a (standard) rule and keep the solder mask expansion per pad set to automatic.

3) The 3D model is just for you. I do prefer having one from the manufacturer as it can help verify the footprint. However, I have also found many issues with supplier 3D models.
I think that I made about 25% of the 3D models on my board. That includes the model of the part above.
The pick and place machine uses a pick-and-place file.
Body (component) height may help, but it may also be used for the AOI.

[nick38]

Ok, Thanks for your reply. I have some more questions:

1- The S1 pad has a bevel edge on the upper left corner of the "Land Pattern" I cant seem to create this on my footprint. Is there any way to create it? Is it absolutely necesary to make it?
2- What is the purpose of the "Land Pattern Mask" is it to add the solder paste for the stencil?
3- I wasn't able to find the 3D model for this part, so I found one that is very similar but the pads sizes and locations vary a little bit. Is it ok if I use it anyway? is the 3D model used to align the part for the pick and place machine?

[qdrives]

The encircled values are of the center points of the pads.
0 is in the middle of the component (I added a blue cross)

If we assume that all pads align at the outer edge, like marked with the green lines, we can calculate the (vertical) center position of the C pads.



The bottom view gives the physical size of the 'leads' on the component.
The recommended land pattern are the dimensions of the pads on the board. These are usually bigger than the leads on the component.
In most tools it is not needed to design the mask (land patterns mask). In this case, the mask expansion (Altium) is 50um. This value I have as my board rule, so I can keep it set to "rule"

The land patterns should be as viewed from the top. The bottom view is a mirror image.

Pad B is once in the component (0.425x0.45) and pad C is twice (2x) in the component (0.45x0.425).
The 90° rotation --> just swap width and height.

[nick38]

Hi,

I'm trying to create the footprint for this duplexer QPQ1289 in Altium and I have the following doubts: First I'm not sure which drawing I should use. Is it the one that say "Bottom view" or the ones that say "Recommended Land Pattern" and "Recommended Land Pattern Mask" they are on pages 7 and 8 in the datasheet. I'll attach pictures of the drawings with numbers circled in red which I don't understand what they mean. Also, what is the "1x THIS ROTATION" and "2x 90 ROTATION" supposed to mean?


Thanks!