First "real" Kicad Project - small issues

[gildasd]

I've been using three main resources:
- Windsor Schmidt's (WS) channel: https://www.youtube.com/user/TroubleHelix
- Chris Gammel's (CG) channel: https://www.youtube.com/channel/UCkJRycUz2CylxpiP-zMePow
- And searching other threads on this forum
Sadly, some of the critical info I found is about previous versions of Kicad with frustrating differences...

-Firstly, this being my first project that does NOT use a battery, the rules checker does NOT like the 12V power in...
I used CG's Vcc method and I still get the same error, WS skips over this with no info...
Can this be solved by putting a power plug/pins in the schematics?
(See attachment 1)

-The CV PCB hates my guts (and most of my ancestors) and throws error messages galore...
This problem is solved - no chickens were sacrificed - relevant attachments removed.

I'll keep posting problems in this thread as I delve deeper into the void...
The whole schematic (See attachment 2) and in pdf (See attachment 3)



(This is a follow up to a previous thread: https://www.eevblog.com/forum/beginners/filtering-an-output-analoque-rms/msg858052/#msg858052 )

[MarkS]

Where is the 12 volt supply coming in from? You don't have any connectors on the board connecting to the 12 volt bus. Look at the error. How are you driving the 12 volt input?

[ElektroQuark]

Add a "Power Flag" from the power library to both +12V and GND.

[gildasd]

Add a "Power Flag" from the power library to both +12V and GND.

Ok I get it.
Method, go to point 42: http://docs.kicad-pcb.org/en/getting_started_in_kicad.html

[MarkS]

Add a "Power Flag" from the power library to both +12V and GND.

I'm just getting started with KiCAD. You don't need to do that with Eagle. Odd.

[Codemonkey]

I've done a number of boards with KiCad and never had to do this either!

[gildasd]

I've done a number of boards with KiCad and never had to do this either!

Me neither, but all my previous projects were battery powered...

[ElektroQuark]

That's ERC working. You have a pin marked as power input/output. It must be driven with power, you do taht with the power_flag. If you change that pin to be pasive, for example, the error will not kick in again, but you will miss electrical rules check.

[HackedFridgeMagnet]

The reason you only get it sometimes is because it depends on the components you place.

Some components will have pins that are marked as "power out" these nodes dont need separate power flags.
Other components will have pins marked as something else, these would need a power flag if there were other pins connected to the node that were marked as "power in".

So the DRC is trying to check for you, but lets you override it if necessary by adding a power flag.

[gildasd]

I think I have done a mistake on the schematic (there might be a need to buffer between the preamp and the final amplification)...
This is simply an extra quad op amp (one component).
I noticed this after laying out my components in PCB new but before laying out any tracks.
Can I still modifiy my schematic without having to redo the whole component lay out?

[ve7xen]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

[suicidaleggroll]

Yes, you can go back and modify the schematic or footprints as much as you want, at any stage in the design.  Just make your changes, as ve7xen said, do NOT re-number the components, assign your footprints, then in CvPCB read the netlist, and make sure you check the boxes to update footprints (if you changed the footprint for a part) or delete extra footprints (if you deleted a part in the schematic) as necessary.  Nothing will be modified on the board that doesn't have to be.  Your new parts will be placed in the normal spot for new parts, and any parts with an updated footprint will be updated in-place (make sure you re-route any tracks to its pins as necessary).

This is handy when using an MCU with extra GPIOs or using CPLDs or FPGAs.  You can lay out the parts as desired in CvPCB, then go back to your schematic and wire the components up to the pins that are most convenient given your placement.  Got a pair of tracks that would have to hop over each other to get to your MCU, and you don't have any particular reason for them to be routed to the exact pins you have them routing to?  Swap them on your schematic, re-load the netlist in CvPCB, and you're good to go.

I'm often going back and forth between CvPCB and EESchema, making small adjustments here or there to improve signal routing or make things easier.

[gildasd]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

Thanks, that worked fine. 
Another little issue, some ground pads did not connect to ground... Is there a manner to manually force this?
As an example, the middle pad of this TO220 needs to be to GND

[ve7xen]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

Thanks, that worked fine. 
Another little issue, some ground pads did not connect to ground... Is there a manner to manually force this?
As an example, the middle pad of this TO220 needs to be to GND

It may just be that the flood fill hasn't been regenerated since the netlist changed. If you right click around the border of the fill there's an option to regenerate the fill (I don't remember exactly what it is), which will recalculate it and if it's the same net as the pin, connect it. I usually just turn the fills off until very late in layout, they just get in the way.

[suicidaleggroll]

Another possibility is the clearance on the fill is set too large for it to be able to reach the middle pin without violating the clearance to the surrounding pins (doubtful in this case, but it could happen elsewhere).  You can modify the properties of the fill to reduce the clearance, which will let it reach places it otherwise couldn't.

[gildasd]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

Thanks, that worked fine. 
Another little issue, some ground pads did not connect to ground... Is there a manner to manually force this?
As an example, the middle pad of this TO220 needs to be to GND

It may just be that the flood fill hasn't been regenerated since the netlist changed. If you right click around the border of the fill there's an option to regenerate the fill (I don't remember exactly what it is), which will recalculate it and if it's the same net as the pin, connect it. I usually just turn the fills off until very late in layout, they just get in the way.

Magic, you are magic!

[langwadt]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

Thanks, that worked fine. 
Another little issue, some ground pads did not connect to ground... Is there a manner to manually force this?
As an example, the middle pad of this TO220 needs to be to GND

is the pin connected to ground in your schematic?

the resolution is bit low, but if it's the regulator in top left corner of "Question007-All.jpg" it looks like you didn't

[gildasd]

If I understand you correctly, then yes you can. If you modify the schematic and save a new netlist file (be careful not to renumber the components though...), then load the netlist in the PCB editor, it will keep everything where you put it and only add new components. There are a couple of options related to this in the read netlist dialog box.

Thanks, that worked fine. 
Another little issue, some ground pads did not connect to ground... Is there a manner to manually force this?
As an example, the middle pad of this TO220 needs to be to GND

Yup, I had not grasped the "reflow fill after netlist modification".
The File is done, I'll check it again tomorrow before sending it.
Thanks.
is the pin connected to ground in your schematic?

the resolution is bit low, but if it's the regulator in top left corner of "Question007-All.jpg" it looks like you didn't

[gildasd]

Done!
I tried to use all the advice on this thread and other noob threads.
This is the third iteration, I could not get the Autoroute do work properly. Looked like a robot had a bad case of VIAs poisoning.
In the end, I did it all by hand, turning components over as needed.
Paid particular attention to not leave any "islands" of 9V or GND, the auto-checker missed most of the large  - but spotted all the small.

Oddly, I found it much easier to start on the output, never would have guessed.
Image 1: Component layout.
Image 2: 9V layer
Image 3: Gnd.
Image 4: Schematics.

Thanks to all!

[Godzil]

Your non power track seems really really thin, what setting have you used?

[gildasd]

To compare, these are the Gerbers with partial Autoroute.
The power was done by hand and then auto-routed. Then modified to fit inside the board.
I had to hand this in, probably will get a good mark, but no way I'm sending this to manufacturing!
(Hence the version above)

[gildasd]

Your non power track seems really really thin, what setting have you used?

0.25 (default setting), should I change this?

[Godzil]

Strictly speaking, it would depends on your board manufacturer and their capabilities.

As your design is through hole only I would have use larger track, but I don't think it make a big difference unless large current run through the tracks

[gildasd]

The worst case is 9V at 0.07Amps - but it would need a major short to do that.
The output is limited by 4V Zeners and the input power by a fuse.
I'll check the manufacturer http://www.mijnprintplaat.nl/prototype-printplaat-laten-maken/

Edit; error change in the URL


    Minimale baanbreedte > 6mil (> 0,153mm) trace min: 1.53mm
    Minimale afstand tussen banen/pads > 6 mil (> 0,153mm) Pad to pad min: 1.53
    Minimale afmetingen > 10x10mm min pcb size 10*10mm
    Minimale boordiameter (via's) 0.4mm min via diam: 0.4mm

[gildasd]

Due to price constraints (95€ vs 40€) I've gone single sided...
And it was HARD, here it is before optimising the GND filling.

[c4757p]

Where on earth are you having the PCB made, where double-sided costs extra (and more than twice as much!?)

[Godzil]

On factory where they have lines that can only do single sided PCBs (there are some)

[gildasd]

On factory where they have lines that can only do single sided PCBs (there are some)

http://www.mijnprintplaat.nl/prototype-printplaat-laten-maken/
It's the best I've found so far...
If you know anything better in Europe, I would very much like that info...

I've optimised as far I can... But hard to do better on a single layer! 

[c4757p]

Is it really hard for Europeans to order PCBs from China or something? I keep seeing Europeans stuck with some really shitty deal on PCBs because they're only looking at EU fabs and all the offerings there suck...

Nice job with the single-sided layout, though.

[gildasd]

https://www.pcb-pool.com/ppfr/order_productconfiguration_js.html
69€ (Delivery?)
http://www.makepcb.com/
44.58 Delivered.
http://www.2cisa.com/index.php?com=presupuestos&promoxpress=0
218€ 

[gildasd]

Is it really hard for Europeans to order PCBs from China or something? I keep seeing Europeans stuck with some really shitty deal on PCBs because they're only looking at EU fabs and all the offerings there suck...

Nice job with the single-sided layout, though.

I've been burnt a few times by Chinese companies, so unless they come HIGHLY recommended, they don't exist...
And we (usually) pay customs and VAT (20% min).
Some Euro factories are also running to capacity, so the only way they can increase profit is to increase price.
I used to order stuff at https://www.olimex.com/PCB/ (i think) but they are refusing work right now...

THe single sided was an exercise in madness!

[Godzil]

I can recommend Seeedstudio as a Chinese manufacturer for PCB.

Or you can also use the services from OSHPark, really competent people, production done really quickly, and made in the US!

I've never had to pay any taxes from my stuff coming from seeed or OSHPark

[gildasd]

I can recommend Seeedstudio as a Chinese manufacturer for PCB.

Or you can also use the services from OSHPark, really competent people, production done really quickly, and made in the US!

I've never had to pay any taxes from my stuff coming from seeed or OSHPark

I'll check them out. Thanks.

Two years ago I bought a nice "kid carrier" backpack in the US. It's a model not distributed in Europe. I paid about 60% extra in import duties and VAT and had to wait 2 weeks... So yeah, sometimes you're lucky, sometimes not.

[langwadt]

I can recommend Seeedstudio as a Chinese manufacturer for PCB.

Or you can also use the services from OSHPark, really competent people, production done really quickly, and made in the US!

I've never had to pay any taxes from my stuff coming from seeed or OSHPark

I'll check them out. Thanks.

Two years ago I bought a nice "kid carrier" backpack in the US. It's a model not distributed in Europe. I paid about 60% extra in import duties and VAT and had to wait 2 weeks... So yeah, sometimes you're lucky, sometimes not.

for some strange reason it seem like everything shipped from the US gets caught in customs and you have to pay tax
while things shipped from China just slips past ... 

[gildasd]

Ready to send the Gerbers/order with http://www.makepcb.com/index.php

I'm probably over-worrying, but the info on the required Gerbers is a bit confusing!
They ask for RS-274x compliance, but don't include the extensions:

Extended Gerber RS-274X (double-layer)

• Silkscreen top
• Layout top side
• Solder mask top side
• Layout solder side
• Solder mask solder side
• Drill info
• Drill info (txt)

I understand that as:
• Silkscreen top = .GTO
• Layout top side = .GTL
• Solder mask top side = .GTS
• Layout solder side = .GBL
• Solder mask solder side = .GBS
• Drill info = .DRL or should it be the .GBR
• Drill info (txt) = .TXT (renamed .DRL)

The lot was checked with GC-prevue and got no errors on any layer.
Any input would be great!

[gildasd]

Received the PCB's today.
Sooo pretty, hope I don't have to bodge anything.

Thanks to all that helped, if anybody would have told me that I could make a rather complex PCB three years ago!

Better go check to BOM...