Capacitive Touch, track pad design (capacitve array)

[Marlon.l]

How would you create a diamond tiled capacitive array for track pad tracking schematic and board design?

I am interested in creating a trackpad 5 cm by 5 cm. I am new to eagle and I don't know how to create easily a pattern for capacitve touch.

I have read around and a suitable diamond dimensions (square antenna) should be 4.5mm by 4.5 mm with a 0.5 mm gap between rows and columns.

the row capacitve antennas could be joined by traces or vias the smaller the routing the better (to prevent interference) .

see similar to https://itp.nyu.edu/archive/physcomp-spring2014/sensors/Reports/Trackpad.html

and

https://www.microchip.com/DevelopmentTools/ProductDetails/DM160219

[Marlon.l]

How would you create a diamond tiled capacitive array for track pad tracking schematic and board design?

I am interested in creating a trackpad 5 cm by 5 cm. I am new to eagle and I don't know how to create easily a pattern for capacitve touch.

I have read around and a suitable diamond dimensions (square antenna) should be 4.5mm by 4.5 mm with a 0.5 mm gap between rows and columns.

the row capacitve antennas could be joined by traces or vias the smaller the routing the better (to prevent interference) .

see similar to https://itp.nyu.edu/archive/physcomp-spring2014/sensors/Reports/Trackpad.html

and

https://www.microchip.com/DevelopmentTools/ProductDetails/DM160219

[JamesLE32J · Accepted solution]

Hi Marlon,

Using your first example I would achieve the footprint with the following steps:

- Create a SMD pad with your desired dimension of 4.5mm x 4.5mm and place this on the Top Copper layer.

- Rotate this pad by 45 degrees.

- Use the Pattern tool to repeat this pad in the X direction with the desired spacing.

- Use the Pattern tool to repeat in the Y direction.

- Use the Line tool to join the pads on the Top Copper layer.

Repeat the above steps for the Bottom Layer patterns.

Some fine tuning will be needed but you'd get there with those steps.

[JamesLE32J · Accepted solution]

Hi Marlon,

Using your first example I would achieve the footprint with the following steps:

- Create a SMD pad with your desired dimension of 4.5mm x 4.5mm and place this on the Top Copper layer.

- Rotate this pad by 45 degrees.

- Use the Pattern tool to repeat this pad in the X direction with the desired spacing.

- Use the Pattern tool to repeat in the Y direction.

- Use the Line tool to join the pads on the Top Copper layer.

Repeat the above steps for the Bottom Layer patterns.

Some fine tuning will be needed but you'd get there with those steps.

[Marlon.l]

I have now tried various methods. This answer isn't as straight forward as I thought out to be.

If you make a SMD node as a device/library. you have to then create a pattern in the schematic. This then is generated into the board, which means you have to manually place them, which is very difficult.

if you create a pattern of SMD in the device, you run into issue of wiring and routing during board placement. This also means it is difficult to scale the amount in the later schematic and board phase.

I tried to create single SMD to wire to an array of rectangular elements, Which I believed would of solve the issue of scaling and wiring in the schematic and board phase. it does not. it's near impossible to create a rectangle as it's dimensions are defined by coordinates.

When creating SMD in the device phase it is also very difficult defining dimensions of a pattern.

[Marlon.l]

I have now tried various methods. This answer isn't as straight forward as I thought out to be.

If you make a SMD node as a device/library. you have to then create a pattern in the schematic. This then is generated into the board, which means you have to manually place them, which is very difficult.

if you create a pattern of SMD in the device, you run into issue of wiring and routing during board placement. This also means it is difficult to scale the amount in the later schematic and board phase.

I tried to create single SMD to wire to an array of rectangular elements, Which I believed would of solve the issue of scaling and wiring in the schematic and board phase. it does not. it's near impossible to create a rectangle as it's dimensions are defined by coordinates.

When creating SMD in the device phase it is also very difficult defining dimensions of a pattern.

[JamesLE32J]

Hi Marlon,

I didn't mean to create an SMD device.  You can create a pad using the 'smd' tool in the footprint editor.

My procedure is:

> New footprint named "CAPACITIVE_TOUCH"

> The footprint editor opens.

> smd tool and drop a pad at x,y 0,0

> Change dimesions of this pad to 4.5x4.5mm

> Use rotate Tool and rotate pad by 45 degrees.

> Use Pattern tool to create a linear pattern with 6.86mm spacing (or you can change the grid to 6.86mm and copy the original pad 12x spaced at 6.86mm)

> Do the same in the Y direction.

You then name the rows and columns accordingly.

This is then a footprint at the correct scaling and there's no need to scale.

The schematic symbol can be as simple as a connection point to each of the rows and columns depending on how you're connecting it to the rest of your design.

I made this in about 3 minutes:

[JamesLE32J]

Hi Marlon,

I didn't mean to create an SMD device.  You can create a pad using the 'smd' tool in the footprint editor.

My procedure is:

> New footprint named "CAPACITIVE_TOUCH"

> The footprint editor opens.

> smd tool and drop a pad at x,y 0,0

> Change dimesions of this pad to 4.5x4.5mm

> Use rotate Tool and rotate pad by 45 degrees.

> Use Pattern tool to create a linear pattern with 6.86mm spacing (or you can change the grid to 6.86mm and copy the original pad 12x spaced at 6.86mm)

> Do the same in the Y direction.

You then name the rows and columns accordingly.

This is then a footprint at the correct scaling and there's no need to scale.

The schematic symbol can be as simple as a connection point to each of the rows and columns depending on how you're connecting it to the rest of your design.

I made this in about 3 minutes:

[Marlon.l]

I am not too sure what you mean by just the footprint editor. the footprint editor is in the library. so I made a new library. To put something onto the schematic you need a device that is mapped to a footprint. So I made a device, which has to be pinned out to the pads, I see you can amend various pads to a pin. In making a single device, I was able to make a foot print see below. I believe I will have to map out individual pads to pins.

[Marlon.l]

I am not too sure what you mean by just the footprint editor. the footprint editor is in the library. so I made a new library. To put something onto the schematic you need a device that is mapped to a footprint. So I made a device, which has to be pinned out to the pads, I see you can amend various pads to a pin. In making a single device, I was able to make a foot print see below. I believe I will have to map out individual pads to pins.

[JamesLE32J · Accepted solution]

Hi Marlon,

I'm wondering whether you are over thinking it (or am I misunderstanding?).  You don't need to map every pad to a pin.  You only need to map an end pad to a pin.  My schematic symbol may look like this which represents the end points on each row/column:

and I would map each of these pins to a 'pad' on the end of each row/column where the yellow ellipses are in the image below (or just on the first pad):

[JamesLE32J · Accepted solution]

Hi Marlon,

I'm wondering whether you are over thinking it (or am I misunderstanding?).  You don't need to map every pad to a pin.  You only need to map an end pad to a pin.  My schematic symbol may look like this which represents the end points on each row/column:

and I would map each of these pins to a 'pad' on the end of each row/column where the yellow ellipses are in the image below (or just on the first pad):

[Marlon.l · Accepted solution]

Yes that's the best way to do it! I have labelled the nodes with IJK convention each respective node is connected with a line. At the ends of each border node is another smaller SMD labeled with XYZ convention. YL$1 (Y axis, left, number).

I will have to add tags >name and >value.

but as we can see we can add multiple touch zones.

[Marlon.l · Accepted solution]

Yes that's the best way to do it! I have labelled the nodes with IJK convention each respective node is connected with a line. At the ends of each border node is another smaller SMD labeled with XYZ convention. YL$1 (Y axis, left, number).

I will have to add tags >name and >value.

but as we can see we can add multiple touch zones.

[JamesLE32J]

Good job Marlon.  Well done.

[JamesLE32J]

Good job Marlon.  Well done.

[lucas.damrau9PDJ7]

Hello there,
I see u are really into Touchpad design. i was trying to do a rounded pad but i fail with importing it for Footprint maker.
Any tips for doing this ?

[lucas.damrau9PDJ7]

Hello there,
I see u are really into Touchpad design. i was trying to do a rounded pad but i fail with importing it for Footprint maker.
Any tips for doing this ?

[jorge_garcia]

Hi @lucas.damrau9PDJ7 ,

I hope you're doing well. This is a pretty involved shape. I recommend making a circular polygon, and then using cutout polygons to make the voids. The pad shape has rotational symmetry, so you could make enough cutouts to do a quarter of the circle.

Let me know if there's anything else I can do for you.

Best Regards,

[jorge_garcia]

Hi @lucas.damrau9PDJ7 ,

I hope you're doing well. This is a pretty involved shape. I recommend making a circular polygon, and then using cutout polygons to make the voids. The pad shape has rotational symmetry, so you could make enough cutouts to do a quarter of the circle.

Let me know if there's anything else I can do for you.

Best Regards,

[lucas.damrau9PDJ7]

Hey @jorge.garcia,
Thank you for the fast answer i was doing it with the polygon tool because cutout was not working so good. But worked out well.
Greetings Lucas

[lucas.damrau9PDJ7]

Hey @jorge.garcia,
Thank you for the fast answer i was doing it with the polygon tool because cutout was not working so good. But worked out well.
Greetings Lucas