Using board cutout for mounting holes - Page 1
Forum section: electronics / general

author: trevwhite
author_rank: Frequent Contributor
timestamp: March 28, 2017, 11:21:32 am
content: I have a PCB outline complete with mounting hole locations. This was from an imported dwg file. Something I could never do with EasyPC and is great that CS supports it.I managed to define a board outline from the object but when I try to define a board cutout from the mounting hole outlines, I get a polygon type object where I define the outline. I want to define a circle as the cutout outline. I can not find any documentation on this, does anyone know how I can do this?ThanksTrev

author: voltsandjolts
author_rank: Unknown
timestamp: March 28, 2017, 12:13:09 pm
content: For round cut-outs just place a zero size pad with the hole size spec'd as you need. Your fab will choose to drill it or router it depending on size.Non-round cutouts are easy enough to create with Home> Board > Board cutout or Place Solid Regionhttp://documentation.circuitstudio.com/display/CSTU/PCB_Obj-BoardShape((Board+Shape))_CSHowever, I don't see a way to define a region/cutout from existing primitives, such as DXF imported shapes. I guess you can use the imported shape as a template to draw round but a "create region from primitives" would be nice.

author: trevwhite
author_rank: Frequent Contributor
timestamp: March 28, 2017, 12:31:31 pm
content: If the board house decides to drill it then there is also a chance it will be plated. I think it depends on the board house process. But if it is defined as part of the board outline then no chance of being plated I reckon.Also if I want a cutout with rounded ends then there must be a way to do this.

author: voltsandjolts
author_rank: Unknown
timestamp: March 28, 2017, 12:54:11 pm
content: You can double click on a pad and set plated property to false to remove hole from list of plated holes, most fabs should pick up on this, it has always worked for me.In the same menu you can define the pad to be slotted (cutout with rounded ends) or use Home > Board > Board cutout with appropriate placement mode and arc radius.

author: trevwhite
author_rank: Frequent Contributor
timestamp: March 28, 2017, 01:09:31 pm
content: ThanksI created a cutout shape and then right click and properties and was able to edit the angle of the arcs. This created the hole for me. It was a lot more work than just creating a zero hole. Probably will just do a zero hole in future.Thanks for the inform on the slot creation.Trev

author: voltsandjolts
author_rank: Unknown
timestamp: March 28, 2017, 02:54:28 pm
content: Ahaa, found it! CS does include "create region from primitives".Select the primitives you want use as a region/polygon/board cutout (perhaps they were created from a DXF import).At the top right of the CS window is a search box. Type in "convert" and from the list of options select "Convert > Create .... from selected primitives"AFAIK the only way to access this option is through that search box....I wonder if there is anything else useful hidden in there?

author: Zbig
author_rank: Frequent Contributor
timestamp: March 28, 2017, 03:05:10 pm
content: Quote from: voltsandjolts on March 28, 2017, 02:54:28 pmIt's funny to think there's possibly the full-blown Altium Designer engine hidden underneath and the product differentiation is done only by not exposing various more advanced functions in the UI. Like with the panelization functionality shown in the other thread.

author: trevwhite
author_rank: Frequent Contributor
timestamp: March 28, 2017, 03:16:26 pm
content: Quote from: voltsandjolts on March 28, 2017, 02:54:28 pmI was never finding that one! Thanks, thats much better and exactly what I wanted. CS seems to have some really hidden power to it.

author: JamesH-AltiumOfficial
author_rank: Contributor
timestamp: April 01, 2017, 12:34:25 am
content: Indeed there is a lot of power in CircuitStudio under the bonnet so to speak, when using the search box to find commands.Here's a list of some noteworthy ones, including the one from this thread:*While you have a PCB focused, search for the string, and hit Enter to run the following commands:Search for create region: Convert > Create Region from selected primitivesSearch for jump comp: Jump > Component*While you have a PCB Library focused:Search for component wizard: Click on the Tools > Component Wizard option (there is an IPC option but it is not available in CircuitStudio).Search for report: Click on the Reports > Library report to create a Word doc with a picture and information about each footprint.Best regards,James HarrimanAltium