search

devbisme / KiPart

Python package for generating multi-unit schematic symbols for KiCad from a CSV file.
MIT License
174 stars 46 forks source link

Option for origin in the center of the symbol. Help with code branch needed... #60

Closed cnieves1 closed 2 years ago

cnieves1 commented 2 years ago

Kicad library requirement S3.1 requires the origin of the symbol to be in the middle of the symbol:

https://klc.kicad.org/symbol/s3/s3.1/

I don't see any option to have the symbol centered.

Is there any way to do this? Would be hard to add?

Thanks in advance,

cnieves1 commented 2 years ago

Hi, I started to write the code to do this. It is currently at: https://github.com/cnieves1/KiPart/tree/center_symbol

I'm using it with a real CSV, attached: SMARC_pin_table2.csv

I'm not quite happy with the results. I admit that I don't know KiPart internals very well, specially regarding the transforms using to rotate/translate the pins...

The pins are not quite centered in the box.

Another thing I noticed is that I would want to move text positions (datasheets, description, reference and so on) so they are outside the box, but at the time they are added to part_dfn, there is still no calculation of the box... could those be just moved at the end of the calculations?

Could you help me to polish and improve it to an state where it can be merged with master?

Thanks,

devbisme commented 2 years ago

I've downloaded your branch. I'll take a look at it.

devbisme commented 2 years ago

I think you were close! I made some changes and checked it in. Take a look and see if it does what you want.

pip install git+https://github.com/devbisme/KiPart@cnieves1
cnieves1 commented 2 years ago

Hi!, Thanks a lot for taking a look at this!

The output is pretty good. I only found some small things to be improved.

In the image below, I think left and right sides should have their pins aligned, since they have the same number of pins:

imagen

In the image below, apart from using the bundle option, would be possible to reduce the Y size of the symbol? There is enough space for top and bottom pin names between pin names on the left and pin names of the right...

imagen

Thanks again!

devbisme commented 2 years ago

I checked in a new version that fixes the alignment problem. It also adds a new option (scrunch) that will push the left/right pin columns under the top/bottom pin rows. Check it out and let me know.

cnieves1 commented 2 years ago

Seems perfect! I didn't find any problem with the new version, and every symbol is now looking nice! I guess you can now merge this branch into master.

Thanks a lot for your support!!

cnieves1 commented 2 years ago

Mmm.. I tried a merge request at kicad symbols repository and there are issues with the symbols, regarding text size and line widths...

See: https://gitlab.com/kicad/libraries/kicad-symbols/-/merge_requests/3556

It may be worth to modify kioart to stick to Kicad KLC...

Thanks

Carlos

devbisme commented 2 years ago

I changed the box line width and font sizes. Try it and see if it fixes the problem.

cnieves1 commented 2 years ago

I get several issues:

PIN_NAME_OFFSET = 20 # Separation between pin and pin name.

imagen

The beginning of the file is:

EESchema-LIBRARY Version 2.3
DEF SMARC_connector J 0 20 Y Y 11 L N
F0 "J" 0 50 50 H V C CNN
F1 "SMARC_connector" 0 -50 50 H V C CNN
F2 "Connector_Amphenol:Amphenol_10151114-00xxLF_SMARC" 0 -150 50 H I C CNN
F3 "https://sget.org/standards/smarc/" 0 -350 50 H I C CNN
F5 "SMARC connector, https://sget.org/standards/smarc/" 0 -450 50 H I C CNN "desc"

  Violating S3.2 - https://klc.kicad.org/symbol/s3/s3.2/
    Text fields should use a common text size of 50mils
     - Pin GND (P100), text size 50, number size 0
     - Pin GND (P103), text size 50, number size 0
     - Pin GND (P12), text size 50, number size 0
     - Pin GND (P120), text size 50, number size 0
     - Pin GND (P133), text size 50, number size 0
     - Pin GND (P142), text size 50, number size 0
     - Pin VDD_IN (P147), text size 50, number size 0
     - Pin VDD_IN (P148), text size 50, number size 0
     - Pin VDD_IN (P149), text size 50, number size 0
     - Pin GND (P15), text size 50, number size 0
     - Pin VDD_IN (P150), text size 50, number size 0
     - Pin VDD_IN (P151), text size 50, number size 0
     - Pin VDD_IN (P152), text size 50, number size 0
     - Pin VDD_IN (P153), text size 50, number size 0
     - Pin VDD_IN (P154), text size 50, number size 0
     - Pin VDD_IN (P155), text size 50, number size 0
     - Pin VDD_IN (P156), text size 50, number size 0
     - Pin GND (P18), text size 50, number size 0
     - Pin GND (P2), text size 50, number size 0
     - Pin GND (P32), text size 50, number size 0
     - Pin GND (P38), text size 50, number size 0
     - Pin GND (P47), text size 50, number size 0
     - Pin GND (P50), text size 50, number size 0
     - Pin GND (P53), text size 50, number size 0
     - Pin GND (P59), text size 50, number size 0
     - Pin GND (P68), text size 50, number size 0
     - Pin GND (P79), text size 50, number size 0
     - Pin GND (P82), text size 50, number size 0
     - Pin GND (P85), text size 50, number size 0
     - Pin GND (P88), text size 50, number size 0
     - Pin GND (P9), text size 50, number size 0
     - Pin GND (P91), text size 50, number size 0
     - Pin GND (P94), text size 50, number size 0
     - Pin GND (P97), text size 50, number size 0
     - Pin GND (S10), text size 50, number size 0
     - Pin GND (S101), text size 50, number size 0
     - Pin GND (S110), text size 50, number size 0
     - Pin GND (S119), text size 50, number size 0
     - Pin GND (S124), text size 50, number size 0
     - Pin GND (S13), text size 50, number size 0
     - Pin GND (S130), text size 50, number size 0
     - Pin GND (S136), text size 50, number size 0
     - Pin GND (S143), text size 50, number size 0
     - Pin GND (S158), text size 50, number size 0
     - Pin GND (S16), text size 50, number size 0
     - Pin GND (S25), text size 50, number size 0
     - Pin GND (S3), text size 50, number size 0
     - Pin GND (S34), text size 50, number size 0
     - Pin GND (S47), text size 50, number size 0
     - Pin GND (S61), text size 50, number size 0
     - Pin GND (S64), text size 50, number size 0
     - Pin GND (S67), text size 50, number size 0
     - Pin GND (S70), text size 50, number size 0
     - Pin GND (S73), text size 50, number size 0
     - Pin GND (S80), text size 50, number size 0
     - Pin GND (S83), text size 50, number size 0
     - Pin GND (S86), text size 50, number size 0
     - Pin GND (S89), text size 50, number size 0
     - Pin GND (S92), text size 50, number size 0
cnieves1 commented 2 years ago

I have double checked and the off grid pin positions were already yesterday: https://gitlab.com/cnieves1/kicad-symbols/-/jobs/2723281994

devbisme commented 2 years ago

Made commit to address these problems:

cnieves1 commented 2 years ago

Thanks again!

I needed to set description by hand (already reported above).

After this round, the complaints are only regarding small tweaks to symbol centering (https://gitlab.com/cnieves1/kicad-symbols/-/jobs/2742840250):


  Violating S3.1 - https://klc.kicad.org/symbol/s3/s3.1/
    Origin is centered on the middle of the symbol
    Symbol unit 1 slightly off-center
     -   Center calculated @ (0, -50)
    Symbol unit 3 slightly off-center
     -   Center calculated @ (50, 0)
    Symbol unit 6 slightly off-center
     -   Center calculated @ (50, -50)
    Symbol unit 7 slightly off-center
     -   Center calculated @ (0, -50)
    Symbol unit 8 slightly off-center
     -   Center calculated @ (0, -50)
    Symbol unit 9 slightly off-center
     -   Center calculated @ (-50, 0)
    Symbol unit 10 slightly off-center
     -   Center calculated @ (0, -50)
    Symbol unit 11 slightly off-center
     -   Center calculated @ (0, -50)

I don't know how important is this, or if the reviewer would want to fix this...

Anyway, all these changes really improved KiPart... Thanks again for your time!!

devbisme commented 2 years ago

For some symbols, it's mathematically impossible to place all the symbol pins on a 100 mil grid and have the centroid at (0,0). The KLC acknowledges this when it states that some small offset of the centroid from the origin is allowed in order to get the pins on the grid. I don't know why the scripts don't account for this. It's similar to the KLC requirement that pin names be offset between 20 and 50 mils from the pins, but the scripts issue errors if the offset is not exactly 20 mils.

Any way, I'll merge this branch into master and place the new version on PyPi.

cnieves1 commented 2 years ago

I fully agree with you.

Let's see what the reviewer says...

Thanks again for your support!

devbisme commented 2 years ago

Was your footprint accepted? If so, I'll close this issue.

cnieves1 commented 2 years ago

You mean the symbol.... No news from the reviewers yet..

Anyway, the goal of this issue was to be able to have centered symbols according to KLC.

This is already accomplished, so I think this issue can safely be closed.

If there is any issue in the future, I'll get in touch again.

Thanks again for your support!!

dnschneid commented 1 year ago

I'd like to clarify the intent on this, as it looks like no attempt was made to move the fields outside the symbol body. Was this intentional or an oversight? afaikt the KiCad style guide shows fields outside the symbol body in screenshots, but doesn't explicitly require one or the other. It's just weird to me that the centered and non-centered behaviors are different in kipart.

PR to make the field positions consistent: #73