Creating PCB footprint from DXF file

[16bitanalogue]

Hello Altium Experts,

I am stuck and I am stupid. Before I buckle and create my own footprint for a Plastronic's socket, I would like to know if this is possible. It seems so, but I am not sure on the necessary requirements/steps. I am new to Altium, so apologies for the dumb question.

I have attached the DXF file for their 5x5 20QFN. I have tried importing it both as component or primitive, but it simply looks like their own outline drawing. Can someone kindly educate me if I can use this file to create a PCB footprint that I can associate with a schematic symbol?

[Doctorandus_P]

I am stuck and I am stupid.

I will not hold that against you.

"Weird" parts such as these test sockets are one of the reasons that "footprint sites" such as SnapEda, PCBlibraries and UltraLibrarian have a place on the internet. Such sites usually have a database with a million or more footprints, and often they are free to download.

Such companies make money by selling footprint generator software to companies that make parts. I have not checked what such sockets cost, but I assume they are not cheap. And to be fair, here in "The West" I sort of expect the companies who make such parts to have footprints for their own parts available, or work together with at least one of the above mentioned "footprint sites". I suggest you send a mail to Plastronics directly to ask if they have footprint data for their products, and if they don't, ask if they are interested on generating that data.

You can not use such test socket footprints without a PCB, so I am quite sure the footprints already exist, somewhere...
 
I use KiCad myself. In KiCad you can load such a drawing as a "background image", in the footprint editor, and use it as a guide to draw the footprint yourself, but you will have to draw it yourself.

Edit: For vector images, (SVG, DXF) the vectors can also be modified / used for other purposes  (such as for example on the silkscreen (legend) layer. So pretty similar to altium as ajb confirmed below.

[ajb]

it simply looks like their own outline drawing.

That's exactly what it is.  A DXF isn't any kind of PCB footprint file, it's a general purpose 2D* vector file format, generally used for technical drawings. 

In KiCad you can load such a drawing as a "background image", in the footprint editor, and use it as a guide to draw the footprint yourself

You can absolutely do that in Altium, except it imports the dxf objects (lines, arcs, etc) into the footprint or PCB as primitives.  You can select which layers of the dxf end up on which layers of the PCB.  If you wanted to just use the drawing as a reference, you can import the desired geometry onto a spare mechanical layer.  If you wanted to directly use the top view on the silkscreen or on the component outline layers, you can do that too -- either map the layers that way when you import, or move the desired objects to the correct layer after import.  You'll need to create the pads and holes yourself, though. 

I'm not sure I'd bother importing anything from this DXF, though, except maybe the top view onto the component outline layer, and I would extract that from the dxf rather than try to import the whole file as is -- I like AutoCAD LT for this sort of thing, but a lot of vector graphics applications can handle dxfs, IIRC including inkscape which is free.  There are dimensions for all of the pins in the DXF, which I bet is also available as a PDF, so you can use those to create and place the pads/holes appropriately.  Fortunately the pads are in a pretty simple rectangular pattern, so a couple of custom X/Y grids would make it fairly easy to place everything without having to do too much math from the provided dimensions.  If they have a step file, you can then place that to verify against the footprint (or import the DXF for reference, or just print the footprint and drawing 1:1 and hold them up to a window...).

* ok, it CAN be used for 3D, but generally isn't except by people who hate themselves enough to do 3D modeling in AutoCAD

[mengfei]

this could save you some time, you can make a request

https://componentsearchengine.com/part-view/EFM8BB52F32I-QFN20/Silicon%20Labs

https://ad.componentsearchengine.com/part.php?partID=17012210

here's how it might look like
https://www.waveshare.com/qfn20-to-dip20.htm

https://www.smithsinterconnect.com/our-company/who-we-are/our-technology-brands/plastronics/

https://en.aliradar.com/item/1989110065-20LQ50S14040-Plastronics-IC-Test-Socket-0.5mm-Pitch-for-QFN20-MLP20-MLF20-package

[PlainName]

Before I buckle and create my own footprint for a Plastronic's socket ...

As the saying goes: "Give a Man a Fish, and You Feed Him for a Day. Teach a Man To Fish, and You Feed Him for a Lifetime."

I would recommend using this as a learning experience which will continue to benefit you long after you're done with this project. All the dimensional info is in the dxf, and if it were me I'd just use the dimensions for the pads to place them as if they were any other footprint. However, you may find the above suggestions of importing the DXF as a template useful as a shortcut.

What isn't known, or shown, are the pad dimensions - hole diameter, pad diameter, etc. A decent place to assist in working that out could be:

https://www.pcb-3d.com/wordpress/tutorials/how-to-calculate-pth-hole-and-pad-diameter-sizes-according-to-ipc-7251-ipc-2222-and-ipc-2221-standards/

Once the footprint is done, you can use the DXF to verify that everything lines up. A 3D model would be great, but you've probably done well to get this 2D drawing!

[tooki]

I highly recommend asking the manufacturer for a 3D model (STEP file), because they’re a great way to make sure you didn’t mess up the footprint. And they’re useful to make sure you don’t inadvertently have interference with some other part.

[Doctorandus_P]

Before I buckle and create my own footprint for a Plastronic's socket ...

As the saying goes: "Give a Man a Fish, and You Feed Him for a Day. Teach a Man To Fish, and You Feed Him for a Lifetime."

I thought is was:

"Give a man a Fire, and he's warm for a day. Set a man on Fire, and he's warm for the rest of his life."

[PlainName]

That works too

[16bitanalogue]

Hello everyone, I have been MIA.

I won't reply to everyone's comments, but overall I will take the approach creating my own footprint. It was a balance between a quick-and-easy (lazy) solution or take the time and roll my own balanced against schedule. Since additional time has been added to the schedule, I am going to revisit my old OrCAD days by creating my own footprints. I am lucky enough to work in a position that this skill is appreciated and "given time." Some managers however....

I did ask Plasatronics for a symbol and footprint specifically for Altium, but they informed me they do not. It will be a good idea if they have a .STEP file. I would have expected Plastronics to inform me of what they do actually have, but if there is no questions asked then there are no answered received in turn.