Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics 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.

Altium designer area fills, vias and plated edges

Status
Not open for further replies.

argam

Newbie
Joined
Nov 2, 2011
Messages
3
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,325
Hello,

although I have checked the forum a few times I have never posted, but now I have a few issues that I hope you can help me with.

I am working in a small RF board on Altium Designer. This is my first time using this software and there are a few things I don't know how to do or if they can be done or not.

The board is a two layer board where the bottom layer is ground and the top layer the signal layer. I have also covered the top layer empty areas with a ground plane, placing a polygon plane as it is done in this video:
Altium Designer Tutorial: Copper planes and pours - YouTube

Now I wonder how I can place in an automatic way evenly distributed vias to connect the top ground plane with the bottom ground plane... is it possible to do that or do I have to place the vias one by one??

The second question is, the vias I am placing have a cross shape as you can see in the image attached... can I change it so that the vias are connected to the metal completelly?
vias.png

Finally I am trying to bring the signal lines to the edge of the board so that I can put this board on a larger board and connect both through these "plated edge vias". What I try to do is to end a line at the edge of the board with a via, but having the via in the edge so that only half of it remains on the actual board.
edge via.png
As you can see the last via is half way out, and therefore I will be able to put this board over another board and solder this edge to a pad. Is this done correctly or is there a better way to do what I pretend to do??

Thanks in advance,
Marcos.
 

Attachments

  • plated vias.png
    plated vias.png
    12.7 KB · Views: 74

PCBcomponentlibraries

Advanced Member level 4
Joined
Oct 14, 2011
Messages
102
Helped
43
Reputation
86
Reaction score
42
Trophy points
1,308
Location
Cheshire, UK
Activity points
1,809
Hi Argam,

Question 1

I don't think there's a way to place via's automatically. But you can place lot's of via's pretty quickly by copying and paste. When you copy it gives you a pick point, you can use this pick point to choose your grid for the vias. So if you had a row of three vias shift click the last two in the row and use the first for your pick point. If you then use the third via in the row as your place point you then have two extra vias at the correct spacing. Using this over and over you can get quite a large area covered pretty quickly.

Question 2

To change the connect style you need to create a new rule. Design --> Rules then add a new Polygon Connect Style rule by right clicking and selecting new rule. Click on your new rule "PolygonConnect_1" in the top full query box you want to put "isvia". Then change the Connect Style to Direct Connect this will connect all your via's to be directly connected.

If you want to refine the rule further you can put in a second restriction in the bottom full query box. The rules are pretty poweful once you get your head around them.

Question 3

I don't know I've never done this maybe someone else can educate both of us.

Hope this helps,
Chris.
 
  • Like
Reactions: argam

    argam

    Points: 2
    Helpful Answer Positive Rating

argam

Newbie
Joined
Nov 2, 2011
Messages
3
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,325
Thanks a lot for your help, both answers helped a lot. Now I have another question. When I was working with a ground plane (layer stack with two signal layers and a GND plane), the autorouter, whenever there was a pad connected to ground, it used a via to connect it to it. Now, I just removed the ground plane from the board, having two signal layers, top and bottom, and I want to use the bottom layer as a GND plane, having the router to put vias whenever a pad is connected to GND. But istead the autorouter tries to connect all the pads through lines on the top layer...
What I did before was to add a Ground plane to the stack and ignore the bottom signal layer. Is that a fine solution or is there a way to have the board with two layers, and have one act as if it was a ground plane??

Thanks in advance,
Marcos
 

PCBcomponentlibraries

Advanced Member level 4
Joined
Oct 14, 2011
Messages
102
Helped
43
Reputation
86
Reaction score
42
Trophy points
1,308
Location
Cheshire, UK
Activity points
1,809
I'm not sure I don't use the Auto router at all I preffer to track all of the tracks by hand - you know what your getting then.
 

Anonymous_Ricky

Advanced Member level 2
Joined
Dec 26, 2006
Messages
516
Helped
88
Reputation
178
Reaction score
58
Trophy points
1,308
Location
India
Activity points
3,974
For providing plated egdes you can make plated router details and adding same in fabrication details or best will be that you ask your fabricator, as he is the one who should understand what you want to do and if it is understanble to him than you can provide plated edges detail any which way.
Regarding last post I suggest you try making bottom layer as unroutable so that autorouter has only one layer to route and once auto routing is done you can do the same for ground signals by blocking top layer(but fix the all prerouted part so that it is not modified)
 

altium60

Newbie level 1
Joined
Apr 22, 2013
Messages
1
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,286
@argam

I don't know if now it's usefull...

In version 10 there is the feature Via Stitching: **broken link removed**

Luca.

dear Luca,
i have a question about via stitching, i use Altium 2010 but i can't find any tab or sth for this command i searched in the net and i found a video about how to use this command it must be in tools- via stitching but i can't find it in my altium if you know how can i use it or how can i active this command please tell me.
thanks in advance
 

SHABU

Advanced Member level 4
Joined
Feb 29, 2012
Messages
118
Helped
29
Reputation
58
Reaction score
27
Trophy points
1,308
Location
INDIA
Activity points
1,860
Better place some SMD pads at the corners and place the via on SMD pads slightly overlapping at an edge.
So that it will be easier for you to solder both boards.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top