FEDEVEL
Platform forum

Shubham , 12-23-2023, 12:33 PM

I don't know what white circles mean and how to resolve this error.

SirJames , 12-23-2023, 01:37 PM

couldn't that be just hardly visible thin traces inside that pad?
Edit: I dont work with Altium so this is just my guess

Mini , 12-23-2023, 01:41 PM

Seems like you have some clearance error. Anyway if you right click it should show which rule you violate.

Robert Feranec , 12-23-2023, 02:40 PM

as @Mini says, its violation. I also tells e.g. < 5mil (it's less than 5 mils and should be more). This could be also track width violation - too thin track (?) I don't have access to Altium right now, but if you click on Panels button (bottom right corner) and select " .... violations ..." it will list all the violations and you can easily browse through them.

QDrives , 12-23-2023, 09:14 PM

The circles mean there is a clearance constrain violation. One thing I would also expect is the short circuit violation and symbol as shown in my capture. Also note that you have set the solder mask expansion to "rule" for the trace.

QDrives , 12-23-2023, 09:15 PM

One way that may help to make thing more clear is to set transparancy to objects so you see multiple traces over one and another.

Shubham , 12-26-2023, 02:07 PM

I understand that it is a clearance constraint. I had explored and changes the clearance constraints rule but I'm unable to avoid collision between traces and pads.

Shubham , 12-26-2023, 02:15 PM

I'm facing this problem in All nets of the board.

QDrives , 12-26-2023, 07:56 PM

If you face this with all nets, then I think you should:
- Validate your project (in schematic: Project / Validate ... )
- Update the PCB with data from the schematic (In schematic: Design / Update PCB document ...)
- Optionally re-sync your component link (in PCB: Project / Component links)
Or did you set a clearance rule to "same net"? (You should not, at least I cannot think of a reason)

Shubham , 12-27-2023, 05:39 AM

thank you for providing detailed solution. Violations are resolved by selecting same net only and selecting layer

Shubham , 12-27-2023, 07:45 AM

Please help me for one more problem. I'm unable to route this.

Robert Feranec , 12-27-2023, 08:36 AM

try to set smaller minimum track width or clearance, if that helps, it means you may need to create a special rule for this footprint or for the area (room) around the footprint.

QDrives , 12-27-2023, 04:25 PM

Have you got s tiny trace in the pad and clearance rules for traces is bigger than for pads? The arrows point to something that alludes to that.

QDrives , 12-27-2023, 04:26 PM

Why "same net only"? Often, the rules are "Different nets only".

Shubham , 01-04-2024, 08:10 AM

Thank You @Robert Feranec @SirJames @Mini @QDrives for your helpful answers. Now I'm more familiar with Altium.

Shubham , 01-04-2024, 08:16 AM

I had completed a two layer board design. But in this design I had faced the below problems . I selected top layer this polygon (Grey) but it is not in red and turns into gray evem their pads and traces are in grey. Why this occurs and how to resolve this problem.

QDrives , 01-04-2024, 11:54 PM

You could have set the net color of net VBAT to that gray color.
In the PCB panel, select Nets, check that none of the nets have a checkbox in front of it (or select the color you want).

Shubham , 01-10-2024, 01:16 PM

how to update existing footprint with new downloaded footprint from UL

Shubham , 01-10-2024, 01:17 PM

in PCB Project

QDrives , 01-10-2024, 09:14 PM

From the PCB: Tools / Update from PCB libraries.
From the PCB library 1: Right-click on the footprint name (PCB library panel) - select Update PCB with ...
From the PCB library 2: Right-click on the footprint name (PCB library panel) - select Update PCB with All
And if you want to replace the footprint: see picture

Shubham , 01-11-2024, 04:53 AM

thank you @QDrives

Shubham , 01-11-2024, 01:12 PM

what will be the via size of 5A Current and trace width of 110 mils. Please suggest me how to calculate via size based on current and trace width carrying high current for two layer and more. I want to connect top and bottom layer 5Amps i.e. 110 mils width size trace with via

Shubham , 01-11-2024, 01:13 PM

please suggest any online calculator or tool

QDrives , 01-11-2024, 09:55 PM

I do not know any online tool, but PCB toolkit is good. An offline (windows) tool.
Most tools show external layers to be (about) double the current compared to inner layers. This is expected to be incorrect. PCB toolkit has the currents almost identical.
For vias I have one simple rules of thumb -- no more that 1A per via. So a 5A connection would require at least 5 vias.

Robert Feranec , 01-12-2024, 05:10 AM

have a look at saturn pcb software - its free and super useful https://saturnpcb.com/saturn-pcb-toolkit/