A SQAURE NPTH HOLE in ALTIUM DESIGNER

[robertferanec]

chitransh92 I didn't know you can do square holes in Altium. Not sure how it shows up in drill files, but interesting. Thanks for teaching me something new

PS: Example:

[chitransh92]

Hello,
An error that generally people run into is changing the pad shape and not the hole shape.
Attached a reference.

1. Shows a Default round hole and round pad
2. Shows a Square pad and round hole
3. Shows a Square hole and Square pad
4. Shows Square hole NPTH as your need probably

Thank you.

[WhoKnewKnows]

It's going to be difficult to produce an absolutely square hole, because the router tool has some minimum diameter, so I recommend drawing the square with rounded corners with a radius that is equal or greater than the PCB manufacturer's minimum route tool radius.

When generating cam data, be sure to enable routing options including saving route paths files as separate from drill files. Also, set the minimum route tool diameter. Then, when viewing, don't forget to load the route path file(s) along with the drills so you can see the intended results.

The drill file will likely have a drill hit in the square hole area so that the route tool doesn't need to plunge before actually routing the hole.

[robertferanec]

I think, this is what you may need (draw the square shape, select it and use Tools -> Convert -> Create Board Cutout from Selected Primitives):

[caltroniks]

Hello Everyone.

I am trying to make a SQUARE NPTH HOLE in PCB .This hole(opening) is for a light sensor .Light would fall onto the sensor through the opening.

For this i was able to make a SQUARE hole using Hole editor .I did get a NC drill NPTH file for square HOLE. However when the drill file was opened in CAMTASTIC or ViewMate i am getting a round drill hole.
Now normally a PCB fabricator will not have a SQUARE DRILL setup .as far as i know no one would have such as anormal practice.

However can any one share info as to how i can show the SQUARE hole in Gerber or a drill file..?
I am starting out with Altium Designer.
Response much appreciated.

Thank you
A.Calvin