Self Learning Kicad as I design a FDC/IO card

[RickyDean]

Here are a couple of the 3D views of what I have so far. This is almost a completed copy of the original WD2793 Corcomp. Just have some touch up work like trying to find or define the varible resistors footprints and so forth.

[RickyDean]

Does anyone have an idea what the proper name for a variable capacitor, the one called on the Corcomp FDC with the 2793 FDC chip is called and can point me to a footprint for Kicad. It would be the one circled in yellow here.

it would have a value of 4pf to 60pf. It is only two pins. not three as I see them on Mouser.

Edited March 31 by RickyDean

[Stuart]

5 hours ago, RickyDean said:

Does anyone have an idea what the proper name for a variable capacitor, the one called on the Corcomp FDC with the 2793 FDC chip is called and can point me to a footprint for Kicad. It would be the one circled in yellow here.

it would have a value of 4pf to 60pf. It is only two pins. not three as I see them on Mouser.

Usually called a trimmer capacitor. Often has 3 pins for mechanical stability - 2 of the pins are connected together.

[RickyDean]

3 hours ago, Stuart said:

Usually called a trimmer capacitor. Often has 3 pins for mechanical stability - 2 of the pins are connected together.

Okay there are some SMD ones in the Kicad library like  C_Trimmer_Murata_TZC3, I'll use that temporarily till I find the right one. Still trying to find the PAL's or Gal's and have to find out how to add library components.

Edited March 31 by RickyDean
spelling, added content

[RickyDean]

[matthew180]

On 3/31/2024 at 9:13 AM, RickyDean said:

... and have to find out how to add library components.

 

A "library" in KiCAD is currently just a single file that contains symbols.  The file can be anywhere you want.  Footprints are their own files that you put into a folder.  3D models are also their own files that you put into a folder.  If you stick the library file, and footprint / model folders into a parent folder, then you have a self-contained "complete" library that you can move around and / or use with all your designs.  Why multiple symbols are contained in a single file vs. footprints being their own files is probably just legacy.

 

Adding your own components is easy, and I recommend you make your own library to put your parts into rather than mixing them in with the stock libraries.

 

I have a github page for my KiCAD library with some instructions on setting up your own library: https://github.com/dnotq/dnotq_kicad_lib

 

Just substitute your own library name and environment variable with whatever you want for your own use.  Use FreeCAD and the KiCAD-StepUp plug-in to align a STEP model with a footprint.

 

Components are extremely easy in KiCAD (better than other EDA programs I have used).  There are three pieces to a complete component:

 

1. Symbol

2. Footprint

3. 3D model

 

The really nice thing about KiCAD is the symbols are completely separate from the footprints.  This is extremely helpful when you have the same part that is available in many footprints (microcontrollers and FPGAs fall into this category, as do SMD passives like caps and resistors).  You add symbols to your schematic and wire them up.  You then choose the specific footprint to use for each symbol.

 

KiCAD associates symbol pins to footprint pads/holes based on name.  So if your symbol has pins 1, 2, and 3, then those pins will associate with pads named 1, 2, and 3 on a footprint.  Symbol pin names, and footprint pad names do not have to be numeric.  For something like and FPGA, they are usually a alpha-numeric grid, like A1, A2, A3, etc..  As long as a symbol pin name matches a footprint pad name, they will be associated.

 

KiCAD will also associate all footprint pads of the same name, with a symbol pin of the same name.  This is common for things like mechanical shields on connectors.  The shield does not actually have a pin number, but many times you need to tie it to ground.  Pin 0 (zero) it typically used for this.  In the symbol you make as many 0-pins as you want (sometimes you only have 1 pin on the symbol for all the shield pins, or you can have one 0-pin in the symbol for each shield pin; however you like).  Then in the footprint you name all such mechanical pads as 0.  In the schematic you can wire the shield to ground and it will be properly associated to all the footprint mechanical shield mounts; and the PCB editor will show them as tied to ground.

 

You can also make your own symbol and use a stock footprint (KiCAD has thousands for footprints that will cover all the industry standard footprints, and lots that are unique), or make your own footprint (I always make my own, but that is just me).  You can also use a stock symbol and make your own footprint.  It is all up to you.

 

Having a 3D model associated with your footprint is very helpful for the 3D preview / rending of your board.  3D models are not required, but highly recommended.  Most of the footprints that come with KiCAD will have 3D models.  And for your own footprints, you can usually download the STEP model from the manufacturer these days, or find it on SnapEDA.

 

For the variable capacitor, I see two symbols in KiCAD that should work fine for the schematic:

 

1. Device > C_Trim

2. Device > C_Variable

 

Those are two-pin symbols that you can use in your schematic.  The footprint you use for the device depends on what part you actually decide to use.  You can even use a 3-pin footprint with the 2-pin symbol, in which case one of the pins will always just be "not connected".  If ERC or DRC complain too much about it, then you can easily duplicate the stock symbol, add a 3rd pin, and set it to no-connect in the schematic.

[RickyDean]

21 minutes ago, matthew180 said:

 

A "library" in KiCAD is currently just a single file that contains symbols.  The file can be anywhere you want.  Footprints are their own files that you put into a folder.  3D models are also their own files that you put into a folder.  If you stick the library file, and footprint / model folders into a parent folder, then you have a self-contained "complete" library that you can move around and / or use with all your designs.  Why multiple symbols are contained in a single file vs. footprints being their own files is probably just legacy.

 

Adding your own components is easy, and I recommend you make your own library to put your parts into rather than mixing them in with the stock libraries.

 

I have a github page for my KiCAD library with some instructions on setting up your own library: https://github.com/dnotq/dnotq_kicad_lib

 

Just substitute your own library name and environment variable with whatever you want for your own use.  Use FreeCAD and the KiCAD-StepUp plug-in to align a STEP model with a footprint.

 

Components are extremely easy in KiCAD (better than other EDA programs I have used).  There are three pieces to a complete component:

 

1. Symbol

2. Footprint

3. 3D model

 

The really nice thing about KiCAD is the symbols are completely separate from the footprints.  This is extremely helpful when you have the same part that is available in many footprints (microcontrollers and FPGAs fall into this category, as do SMD passives like caps and resistors).  You add symbols to your schematic and wire them up.  You then choose the specific footprint to use for each symbol.

 

KiCAD associates symbol pins to footprint pads/holes based on name.  So if your symbol has pins 1, 2, and 3, then those pins will associate with pads named 1, 2, and 3 on a footprint.  Symbol pin names, and footprint pad names do not have to be numeric.  For something like and FPGA, they are usually a alpha-numeric grid, like A1, A2, A3, etc..  As long as a symbol pin name matches a footprint pad name, they will be associated.

 

KiCAD will also associate all footprint pads of the same name, with a symbol pin of the same name.  This is common for things like mechanical shields on connectors.  The shield does not actually have a pin number, but many times you need to tie it to ground.  Pin 0 (zero) it typically used for this.  In the symbol you make as many 0-pins as you want (sometimes you only have 1 pin on the symbol for all the shield pins, or you can have one 0-pin in the symbol for each shield pin; however you like).  Then in the footprint you name all such mechanical pads as 0.  In the schematic you can wire the shield to ground and it will be properly associated to all the footprint mechanical shield mounts; and the PCB editor will show them as tied to ground.

 

You can also make your own symbol and use a stock footprint (KiCAD has thousands for footprints that will cover all the industry standard footprints, and lots that are unique), or make your own footprint (I always make my own, but that is just me).  You can also use a stock symbol and make your own footprint.  It is all up to you.

 

Having a 3D model associated with your footprint is very helpful for the 3D preview / rending of your board.  3D models are not required, but highly recommended.  Most of the footprints that come with KiCAD will have 3D models.  And for your own footprints, you can usually download the STEP model from the manufacturer these days, or find it on SnapEDA.

 

For the variable capacitor, I see two symbols in KiCAD that should work fine for the schematic:

 

1. Device > C_Trim

2. Device > C_Variable

 

Those are two-pin symbols that you can use in your schematic.  The footprint you use for the device depends on what part you actually decide to use.  You can even use a 3-pin footprint with the 2-pin symbol, in which case one of the pins will always just be "not connected".  If ERC or DRC complain too much about it, then you can easily duplicate the stock symbol, add a 3rd pin, and set it to no-connect in the schematic.

Thanks, that helps a lot.

 

Ricky

[matthew180]

The KiCAD documentation is really up to date since they have money now to pay someone to maintain it.  Also, the forum is very active, as is the KiCAD Discord channel.  There are also a lot of videos on KiCAD popping up due to its increased popularity in the last few years.

 

Don't let yourself get frustrated before asking for help.  Everyone has this idea that components are complicated (probably because they are in other EDA programs), or that things like multiple schematic sheets are also complicated.  Most things in KiCAD are really very straight forward, they just take a little understanding on how things are set up.

 

Components just take an amount of detail, especially in the footprint, and getting the 3D STEP model aligned to the footprint can be a little confusing the first time through.  But none of it is hard, and it does not take long once you get the hang of it.  You will be glad you learned.

 

[+FarmerPotato]

On 3/4/2024 at 11:40 AM, matthew180 said:

chip orientation is secondary to cleaner routing.

In the old days, a wave soldering manual called for chips to face their prow into the wave, rather than get hit broadside.  Arrr.

[matthew180]

Oh, interesting.  If there was a manufacturing reason for a particular orientation then for sure that would take a priority.  I didn't know that.

[RickyDean]

Here is a look at the PCB of the Corcomp WD2793 version. I still have to get footprint definitons for the Gals, 4096, 74LS74, 74HCT123, 74LS38, and the 06, but I think most of the traces and items are defined.

Edited April 11 by RickyDean
added content

[matthew180]

Why is U8 so close to the edge?  You have a ton of unused space on the board, I would keep things well back from the edges.

 

Consider spending some time working on the silk screen to make all the labels big, clear, easily visible, and add any information you need to configure the card.

 

Every component should have a designation, and make sure all pin-1 designators are clear.

 

It is hard to tell, but the input power trace to the regulator looks like any other trace; you are paying for the layer, so use the copper.  Also, the regulator is close to the edge, which I realize is typical, but I never understood why they were done what way.  IIRC, the regulators would also short out to the metal case if assembly was done incorrectly.  No need to perpetuate a problematic design.

 

What trace/space are you using for signals, and what are the specs for the vias?

 

Edit:

These are just my thoughts as I look at the board, they are not intended to be criticism.  Just things you might want to consider.

 

Edited April 12 by matthew180
Intention of post

[RickyDean]

9 hours ago, matthew180 said:

Why is U8 so close to the edge?  You have a ton of unused space on the board, I would keep things well back from the edges.

 

Consider spending some time working on the silk screen to make all the labels big, clear, easily visible, and add any information you need to configure the card.

 

Every component should have a designation, and make sure all pin-1 designators are clear.

 

It is hard to tell, but the input power trace to the regulator looks like any other trace; you are paying for the layer, so use the copper.  Also, the regulator is close to the edge, which I realize is typical, but I never understood why they were done what way.  IIRC, the regulators would also short out to the metal case if assembly was done incorrectly.  No need to perpetuate a problematic design.

 

What trace/space are you using for signals, and what are the specs for the vias?

 

Why the U8 is close?

It is because I'm trying to get all the traces run right first then was going to squeeze everything in to fit. This is just a rendition of the actual Corcomp board and is more to show how everythng fits and connects on the actual board. With some work it may be able to make some production boards, but I am aiming a bit higher.

 

After I get all the rough work done, taking what I'm learning and suggestions like yours, on this one, then I want to take and create a board that incorporates both the WD2793 footpprint and the WD1771/73 footprint, to use either of the FDC chips, or both to possibly make a 8 drive system, as I've seen one person do on a website. That one will have all the IC's laying horizontally instead of  vertically for a different look. As for trace thickness and via size, I haven't really thought to much on that as the first and foremost thing was to get it all accurately looking like a Corcomp and if you compare this to an actual board, it comes close to the looks of that.

 

I haven't found the regualtor footprint for a 7805 yet, so what is there is a temporary footprint till I get the right one and incorporate it, then everything should mesh in with the zones I have created for +5v and GND. It's placement was put there for the regulator to be held down by the clamshell as other TI cards were designed, though mine really isn't taking a clamshell into account. My board outline more resembles @Ksarul's protoboard or the new SCSI board @Shift838 is producing.

 

I think I'm doing well for never having used an Electrical Cad program before, and having only designed one small board that is being produced right now. Realize I am keeping your views in mind and will utilize them in the continuing work on these cards and I appreciate your insights as an experience designer.

[matthew180]

No need to justify anything, I'm just giving my thoughts as I look at the board.  Apologizes if it came across any differently.

 

Paying attention to your design rules (based heavily on what PCB house you use), and getting them set up first, will make your life much easier in the long run.  Trace / space is a big one, keep-out and distance between components, and via drill to annular ring size are important.

 

Having a clear and detailed silk screen will make your future-self very happy when you go to do assembly and troubleshooting.