Hi,

? ? I need a ground strap so I can connect the signal and power planes at a point of my choosing. In the past it was possible with a bit of messing about to create a component that did this, however I have just had a board come back from manufacture and this time it has failed because the latest kicad 6.0 will not allow GND and GNDA to be connected even with a frigged component, see below.. Can someone please tell me how to do this in Kicad, its a real nuisance not being able to do this easily as its a feature all other CAD systems have.?

? ?

Thanks in advance!

Russ

On 03/11/2022 21:36, russ95462 wrote:

? ? I need a ground strap so I can connect the signal and power planes at a point of my choosing. In the past it was possible with a bit of messing about to create a component that did this, however I have just had a board come back from manufacture and this time it has failed because the latest kicad 6.0 will not allow GND and GNDA to be connected even with a frigged component, see below.. Can someone please tell me how to do this in Kicad, its a real nuisance not being able to do this easily as its a feature all other CAD systems have.

I don't want to sound too critical, but didn't you check the Gerbers before sending them out for PCB manufacture?

--
Regards,
Tony

I usually just use a jumper, or if there is a lot of power, a series of jumpers.

On 11/3/22 16:36, russ95462 wrote:

Hi,
? ? I need a ground strap so I can connect the signal and power planes at a point of my choosing. In the past it was possible with a bit of messing about to create a component that did this, however I have just had a board come back from manufacture and this time it has failed because the latest kicad 6.0 will not allow GND and GNDA to be connected even with a frigged component, see below.. Can someone please tell me how to do this in Kicad, its a real nuisance not being able to do this easily as its a feature all other CAD systems have.

This is an absolutely vital feature for what I'm now doing. I design induction heater boards for my friend's company (fluxeon.com). On one end of the board is the 3.3 volt processor and analog electronics necessary to protect the SiC FETs on a cycle by cycle basis. On the other end is a 10kW Royer-type power oscillator. I must tie GND and PGND (power ground) together at one point.

4 layer board. The outside lower layer is PGND and the inner ground layer is GND. In Eagle where I'm coming from, to tie the two together, I simply lay down 10 vias in two rows of 5 as close together as my board house can handle. On the bottom layer, the solder mask is manually opened up in the software so that paste is applied across all 10 holes. When reflowed, a continuous solder blob covers all 10 holes and fills them with solder. There is no power flowing through this interconnect but it has to be low impedance so the ground voltage will be the same on both sides so, for example, the source current shunt low side will be at the differential amp's ground. I use a differential op-amp for sensing and for sensing the peak voltage across the FET but keeping the two grounds at the same potential makes things more noise-resistant.

My Rome, GA box builder is competitive with the chicoms until I add many thru-hole devices to the board. A jumper would add cost to the board. I run 50 boards as the pilot run and if everything works correctly, they do a production run of 500.

I've been doing electronic design for decades and was an early evangelist for open source. One guiding principle was and should be now is that FOSS software is better than the nearest commercial equivalent. Being able to connect two planes together directly in the software is vital.

I love this product and send money when I can so I'm an absolute supporter of this project. Let's keep it the best out there.

Thanks,
John

--
John DeArmond
jgd@...
jgd@...

"NeonJohn" == NeonJohn <jgd@...> writes:

On 11/3/22 16:36, russ95462 wrote:

Hi,

? ? I need a ground strap so I can connect the signal and power planes
at a point of my choosing. In the past it was possible with a bit of
messing about to create a component that did this, however I have just
had a board come back from manufacture and this time it has failed
because the latest kicad 6.0 will not allow GND and GNDA to be connected
even with a frigged component, see below.. Can someone please tell me
how to do this in Kicad, its a real nuisance not being able to do this
easily as its a feature all other CAD systems have.

This is an absolutely vital feature for what I'm now doing. I design
induction heater boards for my friend's company (fluxeon.com). On one
end of the board is the 3.3 volt processor and analog electronics
necessary to protect the SiC FETs on a cycle by cycle basis. On the
other end is a 10kW Royer-type power oscillator. I must tie GND and
PGND (power ground) together at one point.

4 layer board. The outside lower layer is PGND and the inner ground
layer is GND. In Eagle where I'm coming from, to tie the two together,
I simply lay down 10 vias in two rows of 5 as close together as my board
house can handle. On the bottom layer, the solder mask is manually
opened up in the software so that paste is applied across all 10 holes.
When reflowed, a continuous solder blob covers all 10 holes and fills
them with solder. There is no power flowing through this interconnect
but it has to be low impedance so the ground voltage will be the same on
both sides so, for example, the source current shunt low side will be at
the differential amp's ground. I use a differential op-amp for sensing
and for sensing the peak voltage across the FET but keeping the two
grounds at the same potential makes things more noise-resistant.

Isn't this what a Net-Tie is used for in KiCad?

My Rome, GA box builder is competitive with the chicoms until I add many
thru-hole devices to the board. A jumper would add cost to the board.
I run 50 boards as the pilot run and if everything works correctly, they
do a production run of 500.

I've been doing electronic design for decades and was an early
evangelist for open source. One guiding principle was and should be now
is that FOSS software is better than the nearest commercial equivalent.
Being able to connect two planes together directly in the software is vital.

I love this product and send money when I can so I'm an absolute
supporter of this project. Let's keep it the best out there.

On 11/3/22 23:21, John Stoffel wrote:

"NeonJohn" == NeonJohn <jgd@...> writes:

On 11/3/22 16:36, russ95462 wrote:

Hi,

? ? I need a ground strap so I can connect the signal and power planes
at a point of my choosing. In the past it was possible with a bit of
messing about to create a component that did this, however I have just
had a board come back from manufacture and this time it has failed
because the latest kicad 6.0 will not allow GND and GNDA to be connected
even with a frigged component, see below.. Can someone please tell me
how to do this in Kicad, its a real nuisance not being able to do this
easily as its a feature all other CAD systems have.

Isn't this what a Net-Tie is used for in KiCad?

I'm not yet skilled enough in KiCad to know of that feature. Thanks for the tip.

John


--
John DeArmond
jgd@...
jgd@...

Hi


A "net-tie" is not a Kicad feature!

Its a PCB design feature/technique to be used when one needs to tie 2 nets in a specific point of the board.

It's more common and easy to understand usage is to connect different ground nets in a single point of the board. Like an analog ground and a digital ground, thus reducing the propagation of high frequency noise from the digital systems to the analog part of the circuit.


Best regards

Jorge

That's what I had created and it worked before but now it does not.?

Not so much being uncritical as unhelpful!. DRC checks should have picked it up I had about ten different boards for hobby use, double sided, and its just not worth looking at gerber files manually for errors, I just do not have the time.

开云体育

On 03/11/2022 21:36, russ95462 wrote:

? ? I need a ground strap so I can connect the signal and power planes at a point of my choosing. In the past it was possible with a bit of messing about to create a component that did this, however I have just had a board come back from manufacture and this time it has failed because the latest kicad 6.0 will not allow GND and GNDA to be connected even with a frigged component, see below.. Can someone please tell me how to do this in Kicad, its a real nuisance not being able to do this easily as its a feature all other CAD systems have.

You haven't stated what problem you actually had, but what I suspect happened is that one of the zones didn't connect to one of the pads of your net-tie "frigged component". This is perfectly reasonable because KiCad is only obeying its default design rules, i.e. different nets cannot be connected, or even contravene the minimum clearance rule. All other PCB programs (Protel, Altium, CadStar) that I use would fall foul of this design rule problem, too.

There are several workarounds, some cleaner than others, but all involve some work, for example:

1. Create duplicate Net-tie footprints. One one of them include the shorting copper, on the other delete it. Initially, perform all your layout using the version without the shorting copper. That way you can fill your two ground zones, and they will connect with the respective pads on the net-tie because no design rules are being broken. finally, when all you layout is complete, swap the net-tie footprints so the final state is wit the one with the shorting copper. If you subsequently run the design rule checker, be sure to clear the checkbox "Refill all zones before performing DRC". If you don't, one of the zones will be disconnected. Of course, the error will still be reported by the checker, but you can then decide to ignore it, and then generate your Gerbers.
   
2. This option is technically "purer". You don't need two Net-tie footprints for this option. Instead, you can define a new Net Class called "Common", or any other name that makes sense to you. You do this in the dialogue that opens in the PCB program from: File > Board Setup > Net Classes. Add your two separate "ground" nets to this net class. Then, in the File > Board Setup > Constraints dialogue, set the clearance for "Common" class to zero. This allows the listed nets to be shorted. If you now run the DRC, no errors will result (at least from your "ground" nets).
   

Done!

So, for someone with zero KiCad experience, how do you learn of:
...adding the keywords "net tie"...

There are some subtle features/settings that are hard to pickup. How do you get up to speed with features like this? This might be hard for a hobby user to sort out.

(Currently, I'm just following along until the day KiCad will do what I need on a daily basis...)

This appears to be? the field you need.

Thanks, that is exactly what I needed.

It's always worth checking the Gerbers. Best is if you use a viewer that is unrelated to the layout program you're using.

Thanks. I didn't know about this feature, but I tried it in 6.0.9, and it does work.

The other method of a "Common" net class with a zero clearance rule I described in another message also works and you don't actually need a component - just a track will do.

I understand how hacks/workarounds get implemented. Unfortunatly it is harder for users to find them.

Glad to hear that documentation is getting attention. My biggest trouble with a lot of open source software lack of documentation. There's a lot of great programmers who want to add wonderful/amazing features to software. However there are fewer people to follow that up with documentation/tutorials/videos, etc (There are exceptions to this, of course). And it's certainly a harder task for software that's quickly evolving. Of course with everything, limited budgets and limited people priorities get shifted...

I think the KiCad team is in a unique position (due to autodesk takeover of Eagle), to be making a product for a known target audience. There's certainly a need for this software, and PCB CAD should be a pretty mature technology by now.

Unfortunately my use case requires KiCAD to have some features it does not yet have. I firmly KiCAD believe it WILL where I need it to be, although that may still be a few years out.

Until then, I'll keep watching this list. Picking up tidbits here and there!