Track width and clearance

[asim131]

Dear Members,
I have two queries
First, I am using AD5624RBRMZ-3 but cant connect to its pins as they seems too thin for track width recommended by my PCB manufacturer(min 10 mil).How to cope with this.
Secondly i have changed my default settings for via,track width,clearance etc after i did all the tracking.So how can i apply these new settings to already existing tracks.Do i have to do all the routing again or there is a way to avoid this.

[Rene_Poschl]

@asim131

First, I am using AD5624RBRMZ-3 but cant connect to its pins as they seems too thin for track width recommended by my PCB manufacturer(min 10 mil).How to cope with this.

Choose another manufacturer or chip package. Ask your manufacturer if they can offer smaller features (will cost more). Ask them if there is a way to have smaller feature sizes at some small area.

---

Is this the gullwing (MSOP) package variant? Because that one has 0.5mm pin pitch. From its dimensions i would guess that the pads will be 0.3 or 0.35mm wide leaving at most 0.2mm clearance. (less than your 0.254mm assuming your manufacturer is setting clearance equal to track width.) So i suggest ask them if the clearance can be reduced. (Track with should be ok as is.)

[Detzi]

You may have a look here for another manufacturer (if applicable) 6mil is usually no problem:

A Price Comparison Site for Printed Circuit Boards

Regarding your via track problem. i fear that you have to go over all the traces and manually change them to the desired track width and drill sitze. I do not know a way to group change that attribute. Would be interesting thou if someone knows more.

[Sprig]

@asim131

Do i have to do all the routing again or there is a way to avoid this.

What version of KiCad are you using?

[Rene_Poschl]

@Detzi

Regarding your via track problem. i fear that you have to go over all the traces and manually change them to the desired track width and drill sitze. I do not know a way to group change that attribute. Would be interesting thou if someone knows more.

With version 5.1 (and possibly also 5.0 but i am not sure about that) you can group select tracks and use the properties dialog (shortcut e or right click -> properties) to change all of them at once.

This works on group selected traces or if you use the new selection tools (right click on a track segment -> select -> all of same net / all connected)

Then there also is the edit track and via properties tool found in the edit menu. Here you can select traces by different filters and either set their new value directly or update them to a change in the netclass (So if you use netclasses then you can change the netclass settings afterwards and use that tool to get the traces updated to these settings.)

[apurvdate]

for updating all vias, you can use text editor to modify the .kicad_pcb file
do remember to backup your file before making changes.

[Rene_Poschl]

@apurvdate

for updating all vias, you can use text editor to modify the .kicad_pcb file
do remember to backup your file before making changes.

Why? There are kicad internal tools for that that are much saver. (See the answer i have given above)

[apurvdate]

I know there are options in layout editor. I’m just listing out another possible option. Apparently OP isn’t aware of either options.
Going via text editor has advantage of using find function in case any of the value is left un-edited.

Speaking of text editor way, I have used that method only once during v4.7 that was for changing Silkscreen text size values.