How to adjust or see a track's height (thickness)?

I have a couple of tracks in my design that draw high current (around 10A) so I need them to be wider. I know how to change the track width but I am not sure where to find the track thickness. I need to know the thickness because ampacity of the track depends on cross sectional area of the track so obviously I need to know the track thickness AND width. To be clear, by thickness I am referring to distance between top of the copper track and board surface.

In calculator seems like the default value is 0.035mm but I don’t see that anywhere on PCB layout editor.

Thank you

Current KICAD does not support PCB stackup definition, so you must “manually” communicate “copper weight” (copper thickness) to PCB fab house of your choice.

You might want to double check how pcb manufacturing works :wink:
In standard processes there is not really an option to vary the “height” of single tracks. The only thing you can specify is the copper thickness of a full layer. Which is typically specified by mail (or via the web interface) when ordering the board (the gerber file format does not contain this information. The newer formats do but they are not yet well supported by most manufacturers)

1 Like

Even with 5.99 which has stackup you would have to “manually” communicate the copper thickness - most manufacturers don’t probably just take the stackup file, at least for their cheap offers.

Here’s one famous cheap manufacturer:

And another:

If you are lucky then you get a metric manufacturer which specifies the thickness in micro meter. Otherwise one needs to read up what 1 oz Cu translates to.

It appears that one-half ounce (oz) of copper is about 17.78 microns, which equals 0.01778 mm.

Edit: see the next comment for a more informed table.

Suggest understanding difference between internal and external layers and applying the IPC-2152 spec’s. Google the spec.

Below is screenshot of table for External traces… (i.e., Top and Bottom layers).


To be fair … since the GERBER format doesn’t encode this information you always have to “manually” communicate with the fab house, irrespective of the tool.

The vast majority of the fab houses out there that provide tailored stackup will take the information you provide and use PCB-Polar to capture the stackup.

How you pass the layer stackup and weight information to the fab-house? typically I will use the user layer and scribe the stackup. Likewise provide a fab documentation.

Having a stackup tool within the the PCB tool however is beyond useful for other reasons and the main one is impedance control for high speed signals

The replacements for the gerber format include stackup so you need a way to enter this info into your design tool if you want to be able to create these newer formats

True, ODB++ (or the ISO equiv) does contain more information associated with the stackup beyond the order. That’s obviously futurestate (is ODB++ on the v6 roadmap? if so still over a year away).

If you are using some sort of PCB train the stackup is whatever they provide. if you are after a custom (different thickness on differnt layers) then you would be paying a premium and would be engaging with teh fab and thus would provide some sort of release document

Every data inconsistency leads to errors.
If you have the Stackup defined (one data source), and then place text on the Comments layer, you can make mistake.
If we would have Stackup definition in the project, the stackup data could be used to export metadata for the PCB Fab (if not included in Fab files like next-gen Gerbers).
For example there could be a plugin/option to generate Stackup diagram from the PCB stackup data on the Comments layer, or to some easily readable document like PDF.
It could include all fab-related metadata like material types, thickness, soldermask colors, design limits (cleareances) and many other in simple and consistent way.
The less manual actions, the less room for errors.

I don’t disagree, I have been stating that since this doesn’t exist (and since KiCAD presently only support GERBER2X) such information must be manually communicated to your fab house.

Even with ODB++ the fab houses I use still like a release document including a drill table and stackup information simple because it is an additional cross-check so they are confident they will build against the correct datapack “your ODB++ state you have 2302 0.3mm holes yet your release document state 2303 0.3mm holes, can you confirm”

This type of service is second to none. The fab house I use will even cross-check intentional shorts in the datapack and the design data.

Thanks everyone. I contacted a manufacturer and they said their thickness is 0.0175 which obviously is not going to work for me. Anyone knows a manufacturer that can do at least 0.1mm thick? I guess that translates to 3oz.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.