Doh!

[paulca]

Don't put your dimension drawings on your edge cut layers!

I spotted it only after sending the files.  I thought, "They'll figure it out." and forgot all about it.  Board passed review I paid and then I was staring off into space looking at the website and suddenly went... wait... it's not rectangular!  (The little picture of the board they show you).  Sure enough my board has "wings" in the shape of my dimension lines.  They don't seem to have cut the numbers into the board and they are only billing me for the original board size.

Hopefully it's just the preview on the site and the production engineer will have the sense to lop off the dimension lines before cutting!

I'll find out in a few days.... a week these days probably.  

Worst case I can score with a rule and knife and snap them.

[Psi]

All pcb designers understand the pain of generating gerbers.

The neverending cycle of

1 - Generate gerbers in PCB design software
- Review gerbers in different piece of software
- Find and fix error
- Goto 1

Then when you're finally happy there's nothing more to fix.

1. Sleep on it.
2. Check again the next day and assuming no more issues are found, place your PCB order.

[Kean]

All pcb designers understand the pain of generating gerbers.

The neverending cycle of

1 - Generate gerbers in PCB design software
- Review gerbers in different piece of software
- Find and fix error
- Goto 1

Then when you're finally happy there's nothing more to fix.

1. Sleep on it.
2. Check again the next day and assuming no more issues are found, place your PCB order.

And yet you still only spot an error the day the PCBs finish production (or the day they arrive).

Like you moved a fiducial at the last minute, but it is now directly under some important text.  Speaking from recent experience...

[Psi]

Yep,  it's one of the situations where math breaks down.

You must put in 150% effort, which is already impossible, but when you do it only finds you 98% of the mistakes.

[wraper]

It's an automated preview which often is rendered wrong. Does not show how your PCB will be actually made.

[paulca]

It's an automated preview which often is rendered wrong. Does not show how your PCB will be actually made.

I'm hoping.

[Doctorandus_P]

Do you have a picture of the PCB / preview?
Did you draw the dimension lines outside the PCB?:-DD

My guess is that the area enclosed by the dimension lines will be included in the PCB area, and the edge of the original PCB will be V-scoring.

[paulca]

Board pic attached LOL.

I had a bit of spare board space, considered cut it off and decided to make a funny feature instead.

https://imgur.com/a/GKw9Cl5

[free_electron]

Really ? I don't even bother to check the Gerber. Never had a problem. then again ..
I run full DRC including all manufacturing rules (silk to silk, silk to solder , silk over bare copper , via from pad , via to via, via tenting and many other rules like pad entry and bend distance ) I do not include any "fluff" in the gerber. No dimensions, drill tables, stackups, legends, logos and nothing outside the board contour. My gerber is production ready. It does not need massaging to remove or add anything. There is a separate document that has all that information. The boardshop does not need nor is allowed to modify my artwork. No copper balancing or clipping or other stuff. My libraries are designed so all objects belonging to a footprint (including the silkscreen polarity markers) are contained in the courtyards with the proper sizing so you can place them blindly. Courtyards can touch but not overlap. You cill not have polarity markers too close to each other, or landing on pads from a different component.

This is one of the biggest issues: irellevant data in gerbers files. Talk to your board shop. They HATE all that extra crap in gerber data, simply because they need to put in time to remove that junk. Drill drawings ? nobody has looked at that in the last 30 years. Dimensions in gerber ? why ? The gerber file has the scale in it. it's not like that shit format called DXF (Deficient exchange format) where there is no scale.

Give them the layers they need (copper, soldermaks and silkscreen) , one layer that shows the board outline and cutouts and the drill file(S). NO OTHER GERBER FILES. A separate PDF has the rest in it (layerstack, net-ties and other info they may need) . ANd give them a netlist for electrical test.

[paulca]

Dimensions in gerber ? why ? The gerber file has the scale in it. it's not like that shit format called DXF (Deficient exchange format) where there is no scale.

Because the last thing I do is measure the board to fill in the box on the website.  The KiCad dimension tool is awesome.  I DID select the "User Drawings" layer, however I then had a bit of a fight with it letting me select the locked edge cut.  It would appear in that fight the Edge Cuts layer got selected and the dimensions ended up there.  Not caught by a last minute check of the Gerbers.  Which I didn't check.  In this case it might have saved me.

[free_electron]

Different tool . I just run the board report. Gives me board size, drill hole count and all possible other data i need to fill out the web order

[redkitedesign]

Because the last thing I do is measure the board to fill in the box on the website.

Most PCB shops can deduce the size from the Gerbers you upload. Certainly PCBWay can do that.

[Doctorandus_P]

I always inspect gerber files before sending them, because they represent your PCB in a "different view" and this helps to spot errors that are somewhat masked by the other views of your PCB. I also spend some time reviewing the 3D view. It's especially useful for reviewing the silkscreen texts and whether it's masked by parts or via holes.

[Psi]

I always inspect gerber files before sending them, because they represent your PCB in a "different view" and this helps to spot errors that are somewhat masked by the other views of your PCB. I also spend some time reviewing the 3D view. It's especially useful for reviewing the silkscreen texts and whether it's masked by parts or via holes.

Exactly, it has to 'look different' for problems to become visible because your brain is always trying to 'fill in the blanks' with what it 'expects' to be there rather than what 'actually' is there. 
Same reason why it's so hard to spot your own spelling mistakes. Your brain keeps seeing what you intended to write not what is actually on the page.


Also, using a different piece of software to check helps to ensure there are no gerber incompatibility issues, not so much of an issue now, but I still like to confirm.

And sometimes things are hidden in the PCB software due to layer order that show up when you look through the layers individually.

[asmi]

And yet you still only spot an error the day the PCBs finish production (or the day they arrive).

I often spot issues after I've ordered them and when it's already too late to cancel the order and re-upload the gerbers

[paulca]

Well, the board arrived without wings!  Yeah!

It even fits the intended board "stacking" idea.

Will have to find out what I forgot later when I wire it up.

And...  I think I might need to give that BlackPill a little alcohol bath.  It's covered in dust and crap!

[paulca]

OMG!  It works.  A few oops in the assembly. 

Lesson of the day.  DO NOT assume the notch means pin 1.  Do not assume pin 1 was correctly labeled on the silkscreen.  Had the WS2812 upside down and it was shorting the board in a rather slow and soft way.

That fixed the ESP32 which I'd had a struggle with was "Brownout detection".  On the off chance I pushed the chip hard into the board and it started working.  So... the GND pad on the back was not flowed.  Soaked it far too long in 350C air until I could push it around, then let it cool.   Works perfectly.

Soldered the screen onto the back before I remembered to solder the JST power header on.  Aw well.  I think I can get an iron in between the boards to do that and I have USB or programmer headers for power.

BTW:  This is what it does...  I/NoT MQTT dashboard.

[Swainster]

Nice project! Just commenting to say that for some reason I always thought that the datasheet of ESP32 says that the centre ground pad on the module version is optional. (WROOM modules, that is - I've not used any other ones)

[paulca]

Nice project! Just commenting to say that for some reason I always thought that the datasheet of ESP32 says that the centre ground pad on the module version is optional. (WROOM modules, that is - I've not used any other ones)

Maybe, but something wasn't flowed either way.  The tricky thing I found with the castellated pads is they overlap the PCB pads a lot without a gap between pins.  That concerned me as the usual DIY approach of plaster the pads in paste and hope it all flows onto pads correctly... has a hard job separating the paste that's trapped under the module.  So I scrapped all the paste to the outside of the pads which may have ended up with too little solder on them.  So in addition to reflowing it, I touched up and added a bit of solder around all the pads.

[Swainster]

For protototyping with castellated modules, assuming no ground pad is needed, then I a stick a piece of card under the module and hand solder them. The gap left by the piece of card makes it possible to remove the module using a solder sucker, after I have blown it up... again.

[tszaboo]

Really ? I don't even bother to check the Gerber. Never had a problem. then again ..

That's all nice, until Altium generates you copper layers, where random part of the silkscreen magically gets exported to a copper layer as well, and shorts out a bunch of tracks. Yes, that happened to me. And if you generate again the gerbers all look ok.
Bonus points, because the copper is below the silk, you cannot really se what's going on until you scrape away the silkscreen.

[Infraviolet]

"Board space to let, apply within", might be more than just funny. I've seen some PCB houses like having text in the top copper layer to help the engineers be utterly sure that they are looking at the top layer and that there hasn't been a mirroring accident.

[Feynman]

The boardshop does not need nor is allowed to modify my artwork.

Believe it or not, but the board shop will modify your artwork

And checking the gerbers not at all is just careless. However, I don't see why it should be an "endless cycle", either.
I only look briefly at every single layer with another tool to check for basic things like registration, origin position and if everything "makes sense" generally speaking.

As others have said: Your layout tool might unintentionally obstruct some things. And having a different software interpreting the data as intended, chances are high that there are no sleeping dogs hidden anywhere. But I agree that in this day and age most CAD tools should be pretty stable in generating gerber files. Finding significant errors in the gerbers should be a rare event.

[free_electron]

Believe it or not, but the board shop will modify your artwork

they will modify widths and masks to meet the end criteria. that is part of their process. But i do not let them remove or add anything.
If the design violates one of their rules , or they find an issue they can tell me  , i will fix the PCB and send new artwork. the board needs to match my cad 100%. I've been burned too many times with fixes done on the board that then were forgotten to be patched in cad and they ended up in the next revision. The CAD is the one true source of truth. I've also been burned with fabs adding copper balancing where this was not allowed ( Rf boards, boards with high voltage so their copper thieves basically shot the creepage to pieces. or stackups with other prepregs. I design the board. they make it. If they need to shrink the soldermask to compensate for bleed : fine, go ahead , but i call for 3 mils over copper with a max 2 mil misalignment. Class 3 boards.

And checking the gerbers not at all is just careless.

The board shop will find the issues if it doesn't match the netlist. What will you learn from the gerbers ? Besides , when i say gerber i really mean odb++ and more recently ipc2581. gerber is gone

Your layout tool might unintentionally obstruct some things. And having a different software interpreting the data as intended,

If the libraries are properly designed and the layout follows the rules all will be fine. If your libraries contains silscreen over pads and other shenanigans: fire your librarian.
As for other software interpreting data : that software too can have bugs. Gerber viewers are not cheap. Especially the ones that can do the front-end for the fab and the DFM. There's really only a few out there : Frontline Genesis , Ucamco or Lavenir ( Pentalogix) own that entire market.

I send my design through Valor before generating output as well.

Checking gerber is like checking that your postscript or PCL renders properly before you send it to the printer.

The gerber viewers do not add any value. The frontend processors do as they check against the fab design rules. But you can't do that as you do not have access to the "secret sauce" a fab uses. every fab has their own internal things they do to make your board. There are externally shared rules like track and gap and soldermask opening , but there is internal stuff that they do not share. If your design meets their external stuff there is a very good change it can be built.
Focus on making data that does not need corrections in the fab , like having to clip silkscreen becasue it is too close to other elements.
Also, check for assembly. your design should be solderable... Before you run the bare board : send the masks and padmasters to the assembler to verify for solderability. (or do this in-house using tools like Valor)

[nctnico]

Many board houses show previews of your PCB design as a render nowadays. The one from Eurocircuits is particulary nice to use for a final check (including clearances and so on).