Skip to content
New issue

Have a question about this project? Sign up for a free GitHub account to open an issue and contact its maintainers and the community.

By clicking “Sign up for GitHub”, you agree to our terms of service and privacy statement. We’ll occasionally send you account related emails.

Already on GitHub? Sign in to your account

Knob board rev a sch #210

Closed
wants to merge 6 commits into from
Closed

Conversation

wknutson
Copy link

@wknutson wknutson commented Apr 1, 2022

Schematic is likely function, however it can be simplified. Specifically 2 of the 10 K resistors around the encoder can be removed if the current schematic is functional.

@npetersen2 npetersen2 self-requested a review April 4, 2022 13:55
Copy link
Collaborator

@npetersen2 npetersen2 left a comment

Choose a reason for hiding this comment

The reason will be displayed to describe this comment to others. Learn more.

Thanks @wknutson ! Looking pretty good! A few comments and requests:

  • Change title block to have correct board revision ("A") and your name for Engineer field
  • Add text labels next to DB-9 and DB-15 connects which indicate which AMDC port they connect to, e.g. "To Encoder on AMDC" and "To GPIO on AMDC"
  • DB-9 pin-out looks great; matches AMDC's encoder pin-out
  • DB-15 pin-out looks great; matches AMDC's GPIO pin-out
  • Tidy up designator labels for JP1 and JP2
  • Add part number for C3
  • Add part number for resistors and capacitors supporting the encoder
  • Revise encoder A and B pin's supporting circuitry to match datasheet; encoder pins should not be connect directly to U1, instead should go through a resistor
  • Revise encoder switch support circuitry: think about when the switch goes from closed to open. How long will it take for the input to U1 to see the change? HINT: I believe it was take too long (or, unknown time), so update the circuitry by adding a resistor to fix

wknutson added 2 commits April 8, 2022 10:11
Updated schematic and added notes. Added part numbers for resistors and capacitors, updated footprints, edited title block, and added a 100K resistor.
I've updated the schematic and created a PCB (Board Dimension are about 80mm by 80mm). Parts have been approximately placed on the PCB. All schematic symbols are connected to footprints. A BOM has also been created for a quantity of 1 and 10.
@wknutson
Copy link
Author

Schematic Review PDF

Schematic Review.pdf

Aligned Ground Symbols down, Voltage symbols upwards, removed extra part links for resistors, and changed the 2 2-pin jumpers to 1 3-pin jumper.
@wknutson wknutson requested a review from npetersen2 April 19, 2022 23:08
@npetersen2
Copy link
Collaborator

Thanks @wknutson

I am approving this schematic PR so you can get the PCB layout finished in the new PCB layout PR.

My only comment on your schematic is to potentially change the voltage divider on the encoder output to ensure the ON voltage is sufficiently high. As it is now, the ON voltage from the encoder is just 50%, but by using a 100k resistor, you could increase the ON voltage to ensure U1 sees the voltage transitions as valid.

@npetersen2
Copy link
Collaborator

Please merge this PR and delete this branch. Then, create your new PCB layout branch and PR so we can review your PCB before ordering the board!

I added a GND and 5V pour to the bottom and top layer respectively. I also moved the connectors, rerouted the traces, rounded the edges, and added mounting holes to the board.
@npetersen2 npetersen2 self-requested a review April 26, 2022 16:22
Copy link
Collaborator

@npetersen2 npetersen2 left a comment

Choose a reason for hiding this comment

The reason will be displayed to describe this comment to others. Learn more.

@wknutson I am providing PCB layout comments here on this PR since you are working on the layout.

  • I checked the schematic and it is looking good.
  • Run a Design Rule Check (DRC) in Altium and verify there are no issues. I found an issue with C3 -- there is a small track present which shouldn't be there:

image

  • Add a REVxxxxxxxxA label to your board in the silkscreen
  • Update the board size to be a nice number: it is currently 80mm by 78.957mm, please change to be a round mm size
  • Add a label to the silkscreen near the CON2 and CON1 which indicate which port on the AMDC it should plug into, i.e. "To AMDC Encoder" vs "To AMDC GPIO" etc
  • Add the board outline to the Mechanical 1 layer. Do this via the menu below:

image

Please make these updates ASAP and ping me so we can get this board finalized, merged into develop and ordered! Thanks

@npetersen2
Copy link
Collaborator

npetersen2 commented Apr 27, 2022

Looks like this PR is old and should be closed in favor of the PCB PR: #214 which includes all the same contents.

There will probably be Altium merge conflicts if we merge this PR first and then try to do #214

@elsevers elsevers self-requested a review April 27, 2022 17:35
Copy link
Collaborator

@elsevers elsevers left a comment

Choose a reason for hiding this comment

The reason will be displayed to describe this comment to others. Learn more.

Looking good! Schematic change requests:

  • Add 0's in front of decimal capacitor values -- i.e. 0.1uF
  • Remove Digikey part number above C4

@npetersen2
Copy link
Collaborator

Closing in favor of new PR #214 -- all the changes from this PR have been manually moved to the other PR

@npetersen2 npetersen2 closed this May 2, 2022
@npetersen2 npetersen2 deleted the knob-board-rev-a-sch branch May 2, 2022 14:50
Sign up for free to join this conversation on GitHub. Already have an account? Sign in to comment
Labels
None yet
Projects
None yet
Development

Successfully merging this pull request may close these issues.

4 participants