Opening solder mask over trace segments

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
Tomg
Expert
Posts: 2024
Joined: 20 Jun 2015, 07:39

Opening solder mask over trace segments

#1 Post by Tomg » 27 Mar 2019, 14:46

I don't know if the following method has already been suggested, but here goes anyway. This is a temporary workaround for a missing DipTrace feature (one example is requested here - viewtopic.php?f=8&t=12653&p=26026) that would unmask selected trace segments to allow solder to be added to increase the current rating...

1) Select/highlight the trace segment(s) that need to have the solder mask opened up over them and copy the selection to the clipboard (Ctrl + C).
2) Open a new (blank) instance of the PCB Layout editor and paste the contents of the clipboard into its Design Area (Ctrl + V).
3) Export the newly-pasted trace segments to a DXF file (use the same units) and then close the new instance of the PCB Layout editor without saving the new PCB file.
4) Returning to the original PCB layout, import the new DXF file (DXF Units: (same as file), Import Mode: "Add") into the desired solder mask layer and reposition as needed. You may have to temporarily toggle on/off the Top (or Bottom) copper layer to see the newly-imported solder mask.
5) Use the 3D Preview tool to confirm that the solder mask has been opened up over the desired trace segments.

Just throwing this idea out there for anyone needing to unmask a complex collection of trace segments in one pass. Any and all suggestions/improvements are welcome.

p.s. Here's a more detailed procedure that should automatically place the solder mask openings in the correct location...
1) Select/highlight the trace segments that need to have the solder mask opened up over them and copy the selection to the clipboard (Ctrl + C).
2) Open a new (blank) instance of the PCB Layout editor and paste the contents of the clipboard into the new Design Area (Ctrl + V).
3) In the new PCB layout set the grid size to 3mm, select/highlight all objects (Ctrl + A), press the up-arrow key once and press the left-arrow key once. This should move all objects up 3mm and left 3mm.
4) While still working in the new PCB layout click on "File" in the Main Menu, choose "Export" in the drop-down menu and select "DXF..." in the fly-out menu to bring up the Export DXF dialog window.
5) In the Export DXF dialog window set Units: to "mm", select/highlight the layer on which the objects reside, make sure that the option [x]Use Design Origin is enabled and click on the [Export] button to bring up the Save As dialog window.
6) In the Save As dialog window enter a file name (e.g. "soldermask"), choose a convenient folder (e.g. Desktop) and click on the [Save] button.
7) Close the new instance of the PCB Layout editor without saving the new PCB file.
8) Returning to the original PCB layout, click on "File" in the Main Menu, choose "Import" in the drop-down menu and select "DXF..." in the fly-out menu to bring up the Open dialog window.
9) In the Open dialog window locate and select/highlight the new DXF file (e.g. "soldermask.dxf") and click on the [Open] button to bring up the Import DXF dialog window.
10) In the Import DXF dialog window set DXF Units: to "Millimeters", Import Mode: to "Add", Convert to: to the desired solder mask layer (choose either "Top Mask" or "Bottom Mask") and click on the [Import] button.
11) Use the 3D Preview tool to confirm that the solder mask has been opened up over the desired trace segments.
Tom

Hemant07
Posts: 2
Joined: 27 Jan 2023, 00:23
Location: Bangalore

Re: Opening solder mask over trace segments

#2 Post by Hemant07 » 05 Feb 2023, 22:06

#Thank you so much for this. This is a loophole in the DipTrace to uncover the mask on the traces. I just want to make a few corrections that will give the correct results if used and much more clarity. I partially used your method but instead of DXF format someone should go with Gerber format because the benefits are,
1. In Gerber format you just get the single layer which you can select as a mask and set its position with the traces to put that mask. In DXF format it gives too many layers which make little confusing.
# If someone also wants to select the trace and copper pour gap and remove the mask from it.
Step 1 > Select all the traces which needed to be masked (select segment by segment).
Step 2 > Take the copper pour gap value from the copper pour properties option (ex: 0.15mm in my case).
Step 3 > Paste the traces in the new PCB creation window.
Step 4 > Select each segment of the trace and edit its width value by ((gap in copper pour x 2) +(width of the trace)). For example (0.15mmx2=0.3mm)+(0.5mm).
Step 5 > Set this new value for the segment width value for all the traces (so the mask will cover the trace and copper pour gap).
Step 6 > Export this file in Gerber format (only Gerber file and not Gerber + nc drill).
Step 7 > Import this Gerber file in your existing design by selecting the import mode as "Add", selecting the layer as "Top Mask" and Import.
Step 8 > Adjust the mask layer either manually or with the help of the dimension tool.
Note:- I've used this method for my high-speed RF switch lines to remove solder resist from the trace and also from the trace and copper pour gap.
Hope it helps someone who needs this kind of solution.
Hemant Rajpurohit
Embedded Hardware Engineer

bird
Posts: 70
Joined: 01 Feb 2016, 14:26
Location: TN, USA

Re: Opening solder mask over trace segments

#3 Post by bird » 19 Feb 2023, 07:58

There is a much easier procedure now to open masks for any traces using the polyline tool while providing the needed thickness.
Here is a detail video from Diptrace:

Post Reply