I have an urgent issue where I am unable to find a workable workaround. I need to route some microstrips/CPW towards an IC. The microstript/CPW needs a minimum/specific clearance to the ground plane around it. In the example picture it is 1mm clearance (let’s use this as example). If I connect the trace to a pin the neighboring pins can’t connect anymore since they are inside the clearance of the track. So good so bad. The other option would be to leave the net class of the track as is and create a zone with higher priority around the track which has the desired clearance. Problem: if something comes close to the zone there will be ugly patches without copper and it very time consuming to create an outline with a zone for a single track given a more or less complicated layout. Besides the edges where two zones meet still look very ugly. Is there another work around I haven’t thougt of? Best thing would be to have a clearance option for every track segment like I can set its width or locked status. I know it has been discussed a couple of times but haven’t found any recent progress.
Thanks in advance!
With your settings it’s not possible to route anything to that IC without DRC errors.
The thin red lines around the pads are the clearances, and they go through other pads.
As hmk suggested. One workaround is to work with net ties.
A net tie is a schematic symbol that connects 2 different nets together on the PCB. On the PCB side it’s (currently, workaround) made from SMD pads and some copper sneaked through it.
If you have a lot of these, then It’s probably better to make a custom Footprint (custom net tie?) for this, that on one side fits nicely on the pad of your IC, and on the other side is far enough from it to connect your PCB track with it’s big clearance value.
Yes I know that this kind of routing will throw DRC errors, thats why I started this thread. Net ties are a possibility I considered but since I have PCBs with 50+ RF nets which can have each a different width depending on simulation results, I would have like 100 different net ties in the worst case which is just no option. A very convenient solution in my opinion would be that the clearance of the track ends before it reaches the pad (as the yellow area in my attached picture), but I don’t see a way how to realize that.
Before any other action you need to change the local clearance of the footprint. As I can’t see the global settings I’m not sure if you want to change the global clearance.
Then, it is possible to end the wide track somewhere near the footprint and continue with a narrower track up to the pad. The clearance of the net will be the same for the wide and the narrow segments.
A workaround with some risks: layout all the wide traces with their normal clearance. Then change the clearance to a lower value to let the narrow segments finish the tracks.
Since I can’t change the clearance of a single track segment the clearance of the track “overwrites” the clearance of the pad (see attached image). And I can’t change the clearance of the net in between because if the zones get refilled all the clearances are flooded and I’m back at the beginning.
On your screenshot I see a row of GND pads, and pad 8, with Net-(U101-pad24)
A simple solution for you could be to edit the footprint and extend pad 8 to get your clearance from the other pads.
The KiCad_pcb file has copies of the footprints in them, you can directly edit one of these footprint with [Ctrl + e] to open it in the Footprint editor, and then:
Select the pad (click once on it).
[Ctrl + C] for copy.
Klick again somewhere to select a “reference point”.
[Ctrl + V] to paste.
Select a location for the copy.
In KiCad it is quite normal to have multiple overlapping pads with the same pad number.
Also, if you edit the pad properties, then in the tab “Local Clearance and Settings” you will see that the current value for “Pad clearance” is 0, which means the clearance is inherited from the attached net. If you enter a fixed clearance for the pad then the pad has a different clearance than the net and it won’t interfere with the other nearby pads.
If you have multiple instances of a footprint, then put them in a custom library.
