Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Via setting in Altium 9

Status
Not open for further replies.

sgaltium

Member level 2
Joined
Jun 29, 2010
Messages
44
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,596
Hi,

Altium Designer 9, using auto-routing, anyone know how to set or configure to prevent any via that auto placing on some IC chip area? Because I’m using a IC chip that the chip base design with metal plate, during mount this chip on the board, the base metal plate touched or short circuit with some of the Via.

Thanks.
 

kevin54

Member level 2
Joined
Dec 3, 2010
Messages
45
Helped
30
Reputation
62
Reaction score
29
Trophy points
1,298
Activity points
1,703
I presume there are traces in the area which are covered with solder mask, and your concern is that vias in the same area will short to the metal plate if they have bare copper.

1) You could tent the vias with solder mask, then they would be no different from the traces. You could select the vias in the area (select everything in the area, then right-click on a via and Find similar object, then check the box for "Solder Mask Tenting - Bottom".

2) You could write a design rule to keep vias away from any component with that footprint. Design -> Rules -> Electrical -> Clearance, the right-click and create a new rule with a new name, where First Object (Advanced) Object Kind is Via, and the Second Object (Advanced) Associated with Footprint yourFootprintName, then set the minimum clearance to something big enough to keep vias out of the area.

3) But honestly, I have to tell you, solder mask is intended to prevent solder bridges, it's not meant to be a primary insulation material. You don't just have vias in the area, you also have traces. If solder mask is your strategy to prevent shorts, you need another strategy. Maybe a thin insulation layer, or a metal plate that has clearance above the wiring area. I wouldn't rely on solder mask, it might work on 99% of the boards you build, but you need something that's guaranteed to always work.
 

sgaltium

Member level 2
Joined
Jun 29, 2010
Messages
44
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,596
Thanks kevin54, really appreciate your kindly reply and solutions given,
I will try as your advises.

Cheers.....
 

kevin54

Member level 2
Joined
Dec 3, 2010
Messages
45
Helped
30
Reputation
62
Reaction score
29
Trophy points
1,298
Activity points
1,703
If you can keep everything on the top side (traces and vias), and you just want a bare PCB under the plate, you can place a keepout on the bottom... Place -> Fill -> Tab -> select Bottom Layer and check the "Keepout" box. I think you can even put this in the footprint. That's the best solution if there's room to route everything on the top.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top