This website requires JavaScript.

PCB Design Minesweeping – Common Mistakes When Using Altium Designer

PCB Design Minesweeping – Common Mistakes When Using Altium Designer

Engineering design is a task that emphasizes meticulousness and rigour. It requires consideration from multiple aspects for product demand analysis, design specifications, and functional verification, with the goal of completing the best product with the least amount of work.

"As the saying goes, to do a good job, one must first sharpen one's tools." Speaking of PCB design, it is strongly recommended to understand the Manufacturing & Assembly Capabilities of PCB manufacturers before designing, as well as the rules of PCB design software, to achieve the best design.

Holes / Drilling

1) In the hole attribute menu,“plated”is not checked, causing copper holes to become non-plated after output, leading to open circuits.

2) The design includes blind or buried vias, which we cannot process at the moment, resulting in missing vias.

3) Slot holes designed on the Drill Guide or Drill Drawing layer are not included in Gerber output, leading to missing slot holes.

4) Slots with length and width swaoped, causing abnormal slot hole data output in older versions, insulting in wider slots than intended (newer versions will fix this issue automatically).


1) Designing the text on the copper layer, causing a short circuit on the finished board (Note: Make sure to run DRC before exporting Gerbers).

2) Designing closely spaced pads with thermal relief, leading to open circuits on the finished board (Note: Make sure to run DRC before exporting Gerbers).

3) The size of top and bottom pads being 0, leading to missing pads (It is recommended that the annular ring of through-hole greater than 0.18 mm. They can have different pad sizes on different sides).

4) Uses Solid copper fills in Altium Designer and then importing to Protel 99. Protel 99 does not support this kind of copper fills, and will remove them. Hatched copper pouring should be used in this scenario. It is recommended to use the same software during the entire design cycle to avoid such compatibility problems.

5) Long, narrow traces with hanging ends can cause short circuits due to dry film bridging. It is advised to delete such designs or connect the hanging end with a line width of 5 mil or above. This recommended width also applies when bridging small gaps.

Solder Mask

1) Designing with "Force complete tenting..." selected, causing the manufactured pads to be covered with solder mask ink and therefore not solderable.

2) Mistakenly designing component through-hole pads as vias, and choosing“tented vias”when ordering with PCB design files, resulting in solder pads being tented on the manufactured board.

3) Designing the solder mask expansion as a negative number, causing the manufactured pads to be covered with solder mask (It is generally recommended to use 0.1 mm for solder mask expansion).

Silkscreen / Characters

1) Designing mirrored text on the top layer, resulting in mirrored characters on the finished product (Correct design: top layer characters are upright, bottom layer characters are mirrored, resulting in correct characters on both sides on the finished product).

2) Designing text on top of exposed copper. By default, these will not be printed; if they are required, please specify clearly when ordering and check the production draft to make sure they are present.

3) Silkscreen is only for identification purposes, not for slotting or shaping. Slot holes in the silkscreen layer will not be manufactured (only a frame will be printed as silkscreen).

Outline / Shaping

1) The keepout option is selected for a slot in the design, causing it to be excluded from exported Gerbers (Note: There is no such option in Altium Designer 17 and newer versions, please draw both slot holes and board outlines in the mechanical layer).

2) Designing slot holes and the board outline on different layers, resulting in missing slot holes (Note: Only one unique mechanical layer can be used when ordering, multiple machanical layers are not allowed).

3) Virtual board cutout slot holes can be displayed in 3D preview but are not included in the exported Gerber files; please draw slots with outlines or single lines with width equal to the slot width (minimum slot width is 1 mm).

4) Drawing multiple sizes of holes in the outline layer, leading to ambiguous hole diameter (Note: When the intended size is ambiguous, we use the smallest size for drilling to allow the possibility to rework).

May 20, 2024에 마지막으로 업데이트됨