[cc'ing mezzanine mailing list. As much as possible, we should be discussing these things in public forums]
Hi Sophie. Good work. Comments below.
On Wed, Nov 25, 2015 at 10:15 AM, Sophie Haynes sophie.haynes@linaro.org wrote:
Morning Grant!
So, I had a bit of a nightmare with KiCad the past week (Libraries not being visible, PCBnew being unable to read the netlist, footprints not showing) but it all seems to be working now. The problems seemed to be caused by me stripping back an old template and hashing it to work for me (worried this may be an issue with people using my git project if the rename it?).
Might be. You'll need to experiment with clean installs to see if it causes a problem
Anyway, I've pushed the project to github (https://github.com/sophie-haynes/96boards-mezzanine-project-template.git). If you have a moment, would you be able to look over the schematic? Still not 100% sure if it's correct electronically?
This is good work. I've got lots of comments, but don't let that discourage you. It's to be expected at this stage of a new project.
Comments on the project: - The way most people will use this repository is they will go into their KiCad templates directory ($HOME/kicad/templates) (which may already contain templates for other projects) and do a "git clone <url>" to get the template files. You need to make sure the project is set up to support that. Right now I think the files are two levels too deep. Move all files up so they are at the root of the directory and it should work correctly. (You'll need to experiment though).
I found an example of a Raspberry Pi template that looks like a good example to follow: https://github.com/xesscorp/RPi_Hat_Template
- The project needs a license. Since we want anyone to use this without restriction, I want to use BSD. Create a COPYING file at the root of the directory tree containing the BSD 2-clause license: http://choosealicense.com/licenses/bsd-2-clause/ - Copyright also needs to be specified. The readme file can list your name as the author, but the copyright is held by Linaro, Inc. (Your contract assigns all of your Linaro work to the company)
- Remove the specification pdf. Instead, put a link to the CE spec in the README file. Including the specification messes anyone cloning the project into their templates directory.
- Ask Shovan for a 64x64 png of the 96Boards Logo to put into the meta directory as icon.png.
- I saw something in the KiCad manual about string replacement rules when creating a project from a template, but I couldn't find out what they are. It might be that there is something there that will fix your library problems. Alternately, it might be that if you change the libraries to something other than "mezza.*" that kicad will stop renaming them and make everything work. Again, you'll need to experiment.
Comments on the schematic:
- I would drop the second expansion connector footprint. Just use one and we'll switch the design to using the through-hole stackable connector that I'm using on the new Sensors board. That will make things simpler.
- Add labels for every signal on the expansion connector, not just the ones that are currently in use. It will make it convenient for anyone starting a new project.
- If you flip the USB connector vertically then the shell pins will be on the left and the data signals on the right. That will make the schematic cleaner, and it is what the other mezzanine schematics look like. That way the USB+/- and VBUS signals can go straight into U2 without looping around.
- +1V8 needs to be split into two separate power rails. +1V8 is supplied by the expansion connector, but the USB FTDI device needs to be powered independently. Create a +1V8F rail specifically for the FTDI. - Similarly, rename the +3V3 rail to +3V3F because it is specific to the FTDI chip. That leaves the +3V3 signal available if someone wants a 3.3V rail powered by the expansion connector. Rename +3V3_FTDI to +3V3F also. (I'm suggesting to use F instead of _FTDI simply because that's the terminology we've used on the Sensors schematic. It's not a big deal, but consistency is nice)
- The regulator needs to be swapped out. The CJT1117-3.3 is a 3.3V regulator, but you want to regulate down to 1.8V. There is a XC6206 regulator on the Sensors board schematic that you can use. If fact, looking at the Sensors design is a good guide for what the schematic should look like.
https://github.com/96boards/96boards-sensors
- Rename "GPIO-A" to "GPIO_A" (underscore instead of dash). Every other signal is using the underscore as a separator.
- Drop the level shifter from the schematic for now. We'll talk about adding it back later.
- Wire the FTDI up to UART1 instead of UART0. You don't need to connect the RTS/CTS signals.
- Add a couple of LEDs to CBUS0 and CBUS1 for TX/RX indications
- Add a LED to each of the power rails. People like lights. :-)
- Insert 220R resistors between CBUS2/3 and PWR_BTN/RST_BTN. This gives a bit of protection to the baseboard in the case of something driving the line when it shouldn't.
Comments on the layout: - Move the USB connector to the exact same position as it is on the Sensors board.
- If you're not laying out traces to the components (except for connectors) then delete them from the project entirely. There isn't much value in placing them without traces.
Phew. That looks like a lot, but it is just a lot of little details. When you're finished, we'll need a blog post to publicize the template a bit and also document it on the 96boards website.
Also, is there anything you need me to do in regards to the debugging of the grove board? I was thinking of doing a little post on our findings.
Not just yet. I've got other investigation I need to do. I'd like to have a better resolution before doing another post, but I would like to co-author something with you when I'm done.
g.
On 11/25/2015 10:47 PM, Grant Likely wrote:
[cc'ing mezzanine mailing list. As much as possible, we should be discussing these things in public forums]
Hi Sophie. Good work. Comments below.
On Wed, Nov 25, 2015 at 10:15 AM, Sophie Haynes sophie.haynes@linaro.org wrote:
Morning Grant!
So, I had a bit of a nightmare with KiCad the past week (Libraries not being visible, PCBnew being unable to read the netlist, footprints not showing) but it all seems to be working now. The problems seemed to be caused by me stripping back an old template and hashing it to work for me (worried this may be an issue with people using my git project if the rename it?).
Might be. You'll need to experiment with clean installs to see if it causes a problem
Anyway, I've pushed the project to github (https://github.com/sophie-haynes/96boards-mezzanine-project-template.git). If you have a moment, would you be able to look over the schematic? Still not 100% sure if it's correct electronically?
This is good work. I've got lots of comments, but don't let that discourage you. It's to be expected at this stage of a new project.
Comments on the project:
- The way most people will use this repository is they will go into
their KiCad templates directory ($HOME/kicad/templates) (which may already contain templates for other projects) and do a "git clone <url>" to get the template files. You need to make sure the project is set up to support that. Right now I think the files are two levels too deep. Move all files up so they are at the root of the directory and it should work correctly. (You'll need to experiment though).
I found an example of a Raspberry Pi template that looks like a good example to follow: https://github.com/xesscorp/RPi_Hat_Template
- The project needs a license. Since we want anyone to use this
without restriction, I want to use BSD. Create a COPYING file at the root of the directory tree containing the BSD 2-clause license: http://choosealicense.com/licenses/bsd-2-clause/
- Copyright also needs to be specified. The readme file can list your
name as the author, but the copyright is held by Linaro, Inc. (Your contract assigns all of your Linaro work to the company)
- Remove the specification pdf. Instead, put a link to the CE spec in
the README file. Including the specification messes anyone cloning the project into their templates directory.
- Ask Shovan for a 64x64 png of the 96Boards Logo to put into the meta
directory as icon.png.
I found that the files of the 96Boards Logo are uploaded here. https://www.96boards.org/press/
Akira
- I saw something in the KiCad manual about string replacement rules
when creating a project from a template, but I couldn't find out what they are. It might be that there is something there that will fix your library problems. Alternately, it might be that if you change the libraries to something other than "mezza.*" that kicad will stop renaming them and make everything work. Again, you'll need to experiment.
Comments on the schematic:
- I would drop the second expansion connector footprint. Just use one
and we'll switch the design to using the through-hole stackable connector that I'm using on the new Sensors board. That will make things simpler.
- Add labels for every signal on the expansion connector, not just the
ones that are currently in use. It will make it convenient for anyone starting a new project.
- If you flip the USB connector vertically then the shell pins will be
on the left and the data signals on the right. That will make the schematic cleaner, and it is what the other mezzanine schematics look like. That way the USB+/- and VBUS signals can go straight into U2 without looping around.
- +1V8 needs to be split into two separate power rails. +1V8 is
supplied by the expansion connector, but the USB FTDI device needs to be powered independently. Create a +1V8F rail specifically for the FTDI.
- Similarly, rename the +3V3 rail to +3V3F because it is specific to
the FTDI chip. That leaves the +3V3 signal available if someone wants a 3.3V rail powered by the expansion connector. Rename +3V3_FTDI to +3V3F also. (I'm suggesting to use F instead of _FTDI simply because that's the terminology we've used on the Sensors schematic. It's not a big deal, but consistency is nice)
- The regulator needs to be swapped out. The CJT1117-3.3 is a 3.3V
regulator, but you want to regulate down to 1.8V. There is a XC6206 regulator on the Sensors board schematic that you can use. If fact, looking at the Sensors design is a good guide for what the schematic should look like.
https://github.com/96boards/96boards-sensors
- Rename "GPIO-A" to "GPIO_A" (underscore instead of dash). Every
other signal is using the underscore as a separator.
- Drop the level shifter from the schematic for now. We'll talk about
adding it back later.
- Wire the FTDI up to UART1 instead of UART0. You don't need to
connect the RTS/CTS signals.
Add a couple of LEDs to CBUS0 and CBUS1 for TX/RX indications
Add a LED to each of the power rails. People like lights. :-)
Insert 220R resistors between CBUS2/3 and PWR_BTN/RST_BTN. This
gives a bit of protection to the baseboard in the case of something driving the line when it shouldn't.
Comments on the layout:
- Move the USB connector to the exact same position as it is on the
Sensors board.
- If you're not laying out traces to the components (except for
connectors) then delete them from the project entirely. There isn't much value in placing them without traces.
Phew. That looks like a lot, but it is just a lot of little details. When you're finished, we'll need a blog post to publicize the template a bit and also document it on the 96boards website.
Also, is there anything you need me to do in regards to the debugging of the grove board? I was thinking of doing a little post on our findings.
Not just yet. I've got other investigation I need to do. I'd like to have a better resolution before doing another post, but I would like to co-author something with you when I'm done.
g. _______________________________________________ Mezzanine mailing list Mezzanine@lists.96boards.org https://lists.96boards.org/mailman/listinfo/mezzanine
On 11/25/2015 10:47 PM, Grant Likely wrote:
[cc'ing mezzanine mailing list. As much as possible, we should be discussing these things in public forums]
Hi Sophie. Good work. Comments below.
On Wed, Nov 25, 2015 at 10:15 AM, Sophie Haynes sophie.haynes@linaro.org wrote:
Morning Grant!
So, I had a bit of a nightmare with KiCad the past week (Libraries not being visible, PCBnew being unable to read the netlist, footprints not showing) but it all seems to be working now. The problems seemed to be caused by me stripping back an old template and hashing it to work for me (worried this may be an issue with people using my git project if the rename it?).
Might be. You'll need to experiment with clean installs to see if it causes a problem
Anyway, I've pushed the project to github (https://github.com/sophie-haynes/96boards-mezzanine-project-template.git). If you have a moment, would you be able to look over the schematic? Still not 100% sure if it's correct electronically?
This is good work. I've got lots of comments, but don't let that discourage you. It's to be expected at this stage of a new project.
Comments on the project:
- The way most people will use this repository is they will go into
their KiCad templates directory ($HOME/kicad/templates) (which may already contain templates for other projects) and do a "git clone <url>" to get the template files. You need to make sure the project is set up to support that. Right now I think the files are two levels too deep. Move all files up so they are at the root of the directory and it should work correctly. (You'll need to experiment though).
I found an example of a Raspberry Pi template that looks like a good example to follow: https://github.com/xesscorp/RPi_Hat_Template
- The project needs a license. Since we want anyone to use this
without restriction, I want to use BSD. Create a COPYING file at the root of the directory tree containing the BSD 2-clause license: http://choosealicense.com/licenses/bsd-2-clause/
- Copyright also needs to be specified. The readme file can list your
name as the author, but the copyright is held by Linaro, Inc. (Your contract assigns all of your Linaro work to the company)
- Remove the specification pdf. Instead, put a link to the CE spec in
the README file. Including the specification messes anyone cloning the project into their templates directory.
- Ask Shovan for a 64x64 png of the 96Boards Logo to put into the meta
directory as icon.png.
I found that the files of the 96Boards Logo are uploaded here. https://www.96boards.org/press/
Akira
- I saw something in the KiCad manual about string replacement rules
when creating a project from a template, but I couldn't find out what they are. It might be that there is something there that will fix your library problems. Alternately, it might be that if you change the libraries to something other than "mezza.*" that kicad will stop renaming them and make everything work. Again, you'll need to experiment.
Comments on the schematic:
- I would drop the second expansion connector footprint. Just use one
and we'll switch the design to using the through-hole stackable connector that I'm using on the new Sensors board. That will make things simpler.
- Add labels for every signal on the expansion connector, not just the
ones that are currently in use. It will make it convenient for anyone starting a new project.
- If you flip the USB connector vertically then the shell pins will be
on the left and the data signals on the right. That will make the schematic cleaner, and it is what the other mezzanine schematics look like. That way the USB+/- and VBUS signals can go straight into U2 without looping around.
- +1V8 needs to be split into two separate power rails. +1V8 is
supplied by the expansion connector, but the USB FTDI device needs to be powered independently. Create a +1V8F rail specifically for the FTDI.
- Similarly, rename the +3V3 rail to +3V3F because it is specific to
the FTDI chip. That leaves the +3V3 signal available if someone wants a 3.3V rail powered by the expansion connector. Rename +3V3_FTDI to +3V3F also. (I'm suggesting to use F instead of _FTDI simply because that's the terminology we've used on the Sensors schematic. It's not a big deal, but consistency is nice)
- The regulator needs to be swapped out. The CJT1117-3.3 is a 3.3V
regulator, but you want to regulate down to 1.8V. There is a XC6206 regulator on the Sensors board schematic that you can use. If fact, looking at the Sensors design is a good guide for what the schematic should look like.
https://github.com/96boards/96boards-sensors
- Rename "GPIO-A" to "GPIO_A" (underscore instead of dash). Every
other signal is using the underscore as a separator.
- Drop the level shifter from the schematic for now. We'll talk about
adding it back later.
- Wire the FTDI up to UART1 instead of UART0. You don't need to
connect the RTS/CTS signals.
Add a couple of LEDs to CBUS0 and CBUS1 for TX/RX indications
Add a LED to each of the power rails. People like lights. :-)
Insert 220R resistors between CBUS2/3 and PWR_BTN/RST_BTN. This
gives a bit of protection to the baseboard in the case of something driving the line when it shouldn't.
Comments on the layout:
- Move the USB connector to the exact same position as it is on the
Sensors board.
- If you're not laying out traces to the components (except for
connectors) then delete them from the project entirely. There isn't much value in placing them without traces.
Phew. That looks like a lot, but it is just a lot of little details. When you're finished, we'll need a blog post to publicize the template a bit and also document it on the 96boards website.
Also, is there anything you need me to do in regards to the debugging of the grove board? I was thinking of doing a little post on our findings.
Not just yet. I've got other investigation I need to do. I'd like to have a better resolution before doing another post, but I would like to co-author something with you when I'm done.
g. _______________________________________________ Mezzanine mailing list Mezzanine@lists.96boards.org https://lists.96boards.org/mailman/listinfo/mezzanine
-
Akira Tsukamoto -
Grant Likely