Sl-Alex home lab

Kicad - preparing a PCB for Seeed Studio

Views: 3870Comments: 0
Notes

Translation: RU

When I was busy with one of my projects, I decided to make a PCB. You can say that I could use a breadboard, but I had to make a lot of boards and I didn't want to spend a lot of time with the soldering iron, so my decision was quite predictable: I decided to order a PCB from the factory and place the order at the pretty famous chinese Seeed Studio and I wasn't disappointed with the result. It was pretty easy to prepare the files for the production and place the order.

PCB routing

For my OSH projects I use KiCAD, so in this post I'll describe how to prepare your project and the production files according to the Seeed Studio requirements.

So, first of all we have to setup design rules. Manufacturer requirements can be found here. There are a lot of pictures describing each requirement, so there shouldn't be any questions. Now let's return to the KiCAD and open "Design Rules" menu. Please pay attention that you can set separate rules for each net class. For example, it is possible to set the width for the "power" nets to 2mm, via diameter 1mm and clearance 5mm. When you will start routing these parameters will apply automatically. These settings can be updated "on the fly". For example, if you want to connect the power net to the small pin, you will have to reduce net width.

Check the routing

It can happen that after manual routing you will still have some errors (you can forget to route a net, some polygons can be too close to the other net and so on). In order to find these hidden errors I recommend to use DRC (Design Rules Check). Here you can check the whole PCB against design rules. Pay attention, that the clearance will be checked separately for each net class. If there are some errors, you will be able to highlight them on the board. It looks like this:

Figure 1 — DRC warning. Figure 1 — DRC warning.

If there are no DRC errors than the board is almost ready for the production, but I recommend to check at least some critical places manually.

Pay attention, that Seeed Studio does not make non-plated holes (this additional step was removed from the manufacturing procedure in order to make it cheaper).

Making gerber files

You can find Seeed Studio requirements here. Additionally there is a detailed step-by-step order guide, strongly recommend to read it. Now let's return back to KiCAD. It is very easy to make gerber files. Select menu "File/Plot", select layers, which we want to export, folder for the results, and press "Plot". We need the following layers:

LayerDescription
F.CuCopper (top)
B.CuCopper (bottom)
F.SilkSSilkscreen (top)
B.SilkSSilkscreen (bottom)
F.MaskSoldering mask (top)
B.MaskSoldering mask (bottom)
Edge.CutsBoard edge

Here is a screenshot with my settings.

Figure 2 - Gerber settings. Figure 2 - Gerber settings.

At the last step we have to make a drill file (menu "File/Fabrication outputs/Drill file"). You have to select gerber output format.

Here are my settings.

Figure 3 - Drill file settings. Figure 3 - Drill file settings.

Now let's rename our files according to the manufacturer requirements. My colleague ordered without the renaming, but in order to avoid problems it's better to do it. A small reminder - gerber naming rules can be found here. I'll duplicate them here, but please check that page before placing an order.

File nameNew file name
pcbname-F_Cu.*pcbname.GTL
pcbname-B_Cu.*pcbname.GBL
pcbname-F_SilkS.*pcbname.GTO
pcbname-B_SilkS.*pcbname.GBO
pcbname-F_Mask.*pcbname.GTS
pcbname-B_Mask.*pcbname.GBS
pcbname-Edge_Cuts.*pcbname.GML/GKO
pcbname.drlpcbname.TXT

Final check

OK, gerber files are done, but you want to check them once again, in order to be sure that there are no errors. I recommend to use ZofzPCB. It is free, it allows you to preview your board in 3D and shows you warnings and errors if any. Here is how it looks like:

Figure 4 — Preview in ZofzPCB. Figure 4 — Preview in ZofzPCB.

You can highlight each net separately and see where it is located. In order to do it you need IPC-D-356 file. It is the file, which contains net locations. You can make it in KiCAD via menu "File/Fabrication outputs/IPC-D-356 netlist file". Add it to ZofzPCB and you will be able to highlight each net on the board. Highlighted net softly blinks.

Figure 5 — Highlighted net in ZofzPCB. Figure 5 — Highlighted net in ZofzPCB.

Order

All checks are done successfully, and now it's time to go to the manufacturer website and place an order. Upload a zip with all gerbers here and fill all necessary fields. After uploading a zip you can look at the preview.

This preview does not show complex board edge, only a rectangular one, so don't afraid, everything is OK.

After uploading a zip and after a preview check board size in the appropriate field once again. Sometimes it happens, that this size switches to the bigger values, in this case just update it manually.

Now everything is done, add an order to the cart, pay and wait. In my case it took up to one month from payment till the final delivery, but it depends on a postal service, manufacturing takes about one week, and you will get information about the status of your order by e-mail.

I hope this post was useful. If you have any questions - please ask, I hope I'll be able to answer.