Back to DesignSpark

How to create slotted holes in pads.

Tutorial transferred from old forum with comments. With thanks to MasterFX

This is a short tutorial how to create slotted holes in your PCB Design using DesignSpark PCB. 
DesignSpark PCB doesn't come with a native function to create slotted holes, but it is pretty simple to achieve it with the provided range of functions, and most of the PCB manufacturers are able to use it.


Create a new technology file

The first thing you have to do, is to create a new technology file for the designs which shall use slotted holes.
Select File => New => PCB Technology File


(1) Select "Copy Technology From File". I'm using "metric"
(2) Select default units and precision


Go to the next page and define the number of layers, solder mask etc. In this case I selected 2 Layers and solder mask for top and bottom layer, and covering vias 


Go to the next page an enter the PCB Technology name (in this case I used metric_2layer_mechanical)


Then go to Settings => Design Technology or use shortcut Shift + T


Go to Layer Types and click "Add"


Enter a name for the new layer type, I chose "Mechanical". Set the options according to the following image


After that go to the "Layer" Tab and click "Add"


Select as type the recently added layer type "Mechanical". Also select your preferred color


After that click "OK" and close the Design Technology dialog. Save your design technology file.


Create a new PCB Design 

After creating the technology file you should create a new PCB Design and select the recently created technology file (you can also import it to your existing design using Settings => Technology Transfer)


After that step you design has the new "mechanical" layer.


Create a PCB Symbol

In most cases you want to design a new PCB Symbol which has a slotted holes by default. To create a new Symbol using you new technology file go to File => Libraries
(1) Click on "Tech.Files" and
(2) select the new created technology file
(3) Confirm with the OK Button


After that click on "New Item" (or if you're using the wizard select the technology file in the corresponding dialog)


Draw the "SMD pads" at first preferably. After that draw the first (through hole) pad (1) which should get "slotted". Right click on it and select Properties (2). Set the shape to Oval (3) and adjust the length and width of the pad (4). The length should be at least the length of the slot.


Select the "Add Shape Rectangle" Tool and press "L" (respectively Right Click => Change Layer)


In the next dialog select "Mechanical" as new layer


Then draw a rectangle with the dimensions of the desired slotted hole size.


Save the PCB Symbol and create your component.


Add Component to PCB Design

After creating the PCB Symbol and Component you can add the component to your new/existing PCB Design (with mechanical layer). This may look like this


Create manufacturing Plots

After you finished your design, the last step is to create the manufacturing plots (Gerber’s). Go to "Output => Manufacturing Plots".
Select all the Layers you would like to output as Gerber file. Select the mechanical plot and make sure only the mechanical Layer is selected as "Y"


After pressing "Run" you get all your Plots in a separate file. Normally the manufacturers expect specific file extensions for each layer (e.g. GTL, GBL, GTS, GBS, GTO, GBO). The mechanical layer can be named ".GM" or "GM1" for mechanical or milling layer. You if you are not sure which extensions your manufacturer expects you should ask him and/or clarify what you expect.

If everything was fine the design could look like this:

I hope this tutorial is useful to someone.



Posted by jayx at 16:31 on 01/10/2015

Hi magicpcb The way is exactly the same, however as the output file doesn't carry plating information PCB manufacturers tend assume all holes are plated. If you need some of them not plated, it needs to be described separately and the way depends on PCB manufacturer. It can be another mechanical layer file or some drawing, text description etc.


Posted by magicpcb at 11:58 on 01/10/2015

Great tutorial but it is not clear if this results in plated or unplated slots. How are plated slots achieved?


Posted by michaelcosson at 13:24 on 24/09/2015

What an excellent tutorial! I love that NOTHING was left implied, and that you truly gave step-by-step instructions. This is particularly useful to those of us who are electrical engineers and are just dipping their toe into the mechanical engineering waters! I had searched for the PCB footprint for an "AA" battery contact, which has a 0.5mm x 3.0mm PCB mounting tab. Nothing from the manufacturer. Nothing from DesignSpark. Google is usually my first "go-to", but I didn't do it on this problem, originally. When I did, however, I found your great tutorial. In a matter of about 20 minutes (between reading and actually doing), I came up with the image shown

AA Battery Contact PCB Footprint

Thanks again!


Posted by boss at 18:12 on 28/05/2015

nigelmercier wrote: > How about if making boards at home? Hi Nigel, this raises the question how do you create pcbs at home? The problem with slots for the pcb manufacturers and home users is obviously you can't drill a slot. For home use it's normally two drilled holes and a file whereas the pcb manufacturers mill them and charge a premium for this process.


Posted by nigelmercier at 09:47 on 28/05/2015

How about if making boards at home?


Posted by ahagele at 04:10 on 27/03/2015

Thanks for the tutorial. Does make sense. However how do I get the slots plated? I am putting a standard 2.1mm barrel connector (to use these standard wall power adapters). And the component has blade like components. It required a solid through plated pad to do the job.


Posted by bradlevy at 13:55 on 20/11/2014

Hi JorgeOmar, I didn't author the tutorial - I just answered a few questions about it. It sounds like you are doing things correctly up to the point of generating the manufacturing plots. In the tutorial, the output was to gerber files, and following the procedure shown would produce a gerber file for the mechanical layer in addition to the gerber files for the other layers. The mechanical plot would be mostly empty except for the slots. If you are going to PDF output to see if things look right, you probably want a plot combining the mechanical layer and the top or bottom copper. To achieve that, select Output > Manufacturing Plots from the menu. Click on Top Copper in the Plots: window of the dialog. Then click on the Layers tab of the dialog. The dialog should look something like this:

Double click on the N next to Mechanical in the right-hand box to change it to a Y, so the mechanical layer will be included in the plot of the top copper. -Brad


Posted by boss at 08:33 on 20/11/2014

My understanding is this is purely information for the manufacturer and how to communicate it such that you achieve a slot. It will not visualise any more than the pink slot outline shown, so will be of no use in a pdf. Another method to explore is to place a board outline within the board, which appears as a hole/slot/cut-out.


Posted by jorgeomar at 05:09 on 20/11/2014

Hi Brad Thanks for your contribution...very valuable but I am not getting final results... or at least not able to visualize. Following step by step your tutorial "How to create slotted holes", I managed to create "new technology file" that I names "mech_4layers_mech". I created a "new PCB symbol" using a normal round pad and changing to oval. I created a new component using the new PCB symbol including the Sch symbol. In that case I followed the instruction by adding also a rectangular shape allocated to the new mechanical layer "Mechanical" I added the new component "slotted pad" I added the new layer "Mechanical" into the project. I was then trying to see the slotted pad by printing into pdf but I did not see the plated slotted hole.... what I am doing wrong?.... Of course, I made some many tries that may be my explanation is not accurate enough You explain te process by adding PCB symbol... but I also added a new component... may be this my mistake? Thanks a lot Jorge


Posted by bradlevy at 19:36 on 29/04/2014

@Jan, I think you could start with the default technology file, instead of specifying a specific one (metric). I think the key is that you are starting from the technology you usually use, and adding a mechanical layer to it so your designs based on this new technology file will have a place to put the slot mechanical info. Likewise, some of the other settings in the first few steps can be as needed to match your needs - they don't have to be the same as in the example. -Brad


Posted by jan lichtenbelt at 17:01 on 29/04/2014

The pull down menu is empty, in my case. What to do?


Posted by boss at 12:59 on 29/04/2014

@Jan, It is shown in the pull down menu in the second image. See the red arrow with number 1.


Posted by jan lichtenbelt at 09:08 on 29/04/2014

I get lost already at the first line: (1) Select "Copy Technology From File". I'm using "metric" Where is that metric file?


Posted by ulf herder at 12:12 on 24/05/2013

Hi MasterFX,  thank you for the excellent tutorial! It helped me much for the solder pads of a bridge rectifier. Regards, Ulf


Posted by mikebk at 07:35 on 23/04/2013

Hi MasterFX, excellent tutorial! Many thanks for your contribution Regards, Mike


Posted by rs components support at 21:12 on 16/04/2013

Excellent detailed Knowledge Item MasterFX.  This will be most valuable to many users. Thank you.




Was this article helpful?
0 out of 0 found this helpful
Have more questions? Submit a request


  • 0
    Tom Mattus

    Hello All, I've accomplished making the slotted footprint etc, but when I run the DRC it gives me errors; P-P and T-P, pad to pad and track to pad. Are these to just be ignored because there are pads over pads by design as described in tutorial? 


Please sign in to leave a comment.