Different widths in track

[davorin]

Good afternoon

Doing a simple PCB with 4 Triacs...where the middle pin number 2 is the main line input...so I thought I could easily lay a track between those pins and change the width on the fly:



But as soon the track is connected to the next Triac, the whole track width is switched back to the starting width...and there is just one track now...
Any trick how to do that in KiCAD 9.0?

I remember many years ago that this could been done in OrCAD PCB easily...

[ataradov]

Do two narrow stub segments, copy one of them and change the width of that segment in the properties, move and resize it to touch the other two.

I think the issue here is that KiCad tries to combine aligned segments into one while routing. But if the width is different after a manual change, it won't combine them. I think there may be a setting for that too, so disabling it may help do it on the fly too.

I usually route as is and then just adjust individual segments, but in this case if it optimizes them all into one, since they are linear, it will not work. Temporarily routing them crooked to make sure segments stay separate will work too.

[davorin]

I assume that the track in my case is straight...so it is only one segment.

But good idea for a quick hack (o;

Maybe I'll sign up to the KiCAD forum and ask there if there was a solution..don't believe it can only be done that complicated as OrCAD PCB386 (yeah, I'm old ;o) could do that decades ago (o;

[golden_labels]

Ah, the never ending tug-o-war between freedom and convenience, episode № 68,581,483?

I can’t reproduce the situation in KiCad 9.0.0 or 8.0.8. I can draw one segment, then another, change its width, then finish with another narrower one starting at the other component. They remain separate.

The context menu for traces has a “Break track” action. See if you can draw a single trace and then use this twice to break it into three separate segments.

An alternative option could be drawing a thinner trace and using a fill zone to provide copper area. This will save you headache with clearances. The downside is that fill zones need to be done in the end, as moving footprints is cumbersome with them present.

[davorin]

Just did this screen capture and posted it in the KiCAD forum....gonna test it on Linux tomorrow as well...this is on macOS 15.3.1.

This capture shows how I did the trace two times exactly the same with different outcome:

https://youtu.be/oZfEI_KtMi0

[golden_labels]

Ok, you’re not crazy. I can reproduce this with 9.0.0 if I change track width on the fly.

No idea, how to avoid the situation. It seems disabling snapping (hold Shift while finishing a track) prevents this from happening, but of course we want snapping.

[davorin]

Seems a ticket was created just a week ago:

https://gitlab.com/kicad/code/kicad/-/issues/20031

[PlainName]

Can you not use neckdown for this?

the width will be taken from the netclass of the net being routed (or from any custom design rules that specify a different width for the net, such as inside a neckdown area)

[davorin]

Hmm...never heard of neckdown before.....and don't exactly know what it is (o;

Also what puzzles me is the button right to the track width menu and what it does, nothing can be changed there:

[PlainName]

Don't know about Kicad but in other tools it is where a track automatically reduces to, for instance, fit between pads. The original width would be too wide to go through and transgress some clearance rule, so it is reduced where necessary to ensure the rule remains valid.

What you're doing seems to be the manual version of that, solely to keep away from the neighbouring pads.

Only google result that I can find is to:

https://forum.kicad.info/t/automatic-neckdown/46458/2

where jmk says: "You will find Custom Rules in File > Board Setup > Design Rules. Use the “Syntax Help” to help you create a Custom Rule for Neckdowns." Along with a link to:

https://docs.kicad.org/7.0/en/pcbnew/pcbnew.html#custom_design_rules

[davorin]

Well someone from KiCAD acknowledged that this is a bug introduced in version 9.....so hopefully a new release will be published.

See the youtube link above....

But honestly being a while I did PCB designs and used KiCAD....just started again with it and pumped up my electronic lab as I was just being laid off by my employer after almost 10 years...and with almost 58 chances are almost to zero being employed again....

[Warhawk]

Well someone from KiCAD acknowledged that this is a bug introduced in version 9.....so hopefully a new release will be published.

See the youtube link above....

But honestly being a while I did PCB designs and used KiCAD....just started again with it and pumped up my electronic lab as I was just being laid off by my employer after almost 10 years...and with almost 58 chances are almost to zero being employed again....

davorin, I am sorry to hear that. I cross my fingers for you finding luck somewhere else.

[davorin]

Thanks (o;

Good thing is that I have a lot of free time to finally bring my loads of ideas to live...

Like: Take an old vacuum tube radio...pull out a specific tube, plug in my replacement tube...and you got an internet radio...no changes to the radio needed (o;

Next projects are to turn the Ninja 8-in-1 oven into a SMT reflow oven...and revive my old pick-n-place machine for OpenPNP (o;

[JohanH]

I noticed this as well in version 9. You can work around it. Right click and lock a track, then it's locked in place (and size) and you can add and change other segments. Then you just have to unlock it if you have to move it again.

[JMK]

To change track widths on the fly:

Go to File > Board Setup > Design Rules > Pre-defined Sizes and enter all the track widths you require for this project.

Then, when placing a track, use hotkeys "W" and "Shift + W" to scroll through the list of track widths previously created in the Setup. Each click of the hotkey will increase or decrease the currently being drawn track segment to either the previous or next width in the Pre-defined Track Width list.

[davorin]

Well that I know of (o;

The problem lies with KiCAD 9.0.0 as acknowledged by KiCAD themselves.

[asanx]

Hey! when joining these different sized traces press SHIFT + left mouse click.
It worked for me 

[golden_labels]

Hey! when joining these different sized traces press SHIFT + left mouse click.
It worked for me 

Yes, but as mentioned, it’s only useful if one doesn’t want to have snapping enabled. Shift disables snapping.

[asanx]

I press shift after it has snapped so idk if it matters that much, atleast i can do my work now