Author Topic: multi-layer PCB design and ground free area in Altium  (Read 8512 times)

0 Members and 1 Guest are viewing this topic.

Offline Bud

  • Super Contributor
  • ***
  • Posts: 6877
  • Country: ca
Re: multi-layer PCB design and ground free area in Altium
« Reply #25 on: November 24, 2017, 11:35:39 pm »
:horse:
the top layer has many nets and some of them are sensitive nets as you see above.
the second layer is the ground layer. but under these sensitive nets should be ground free!
3rd layer is the power layer.
4th layer is the solder side.

If I want to pour ground polygon in the second layer, this sensitive area will not be ground free! bcoz the nets are in the top layer and I'm in the second layer!

You have been told to use "polygon pour cutout" . What is the problem ? Learn how to use it.
Facebook-free life and Rigol-free shack.
 

Offline mars01

  • Contributor
  • Posts: 44
  • Country: ro
Re: multi-layer PCB design and ground free area in Altium
« Reply #26 on: November 25, 2017, 09:56:44 pm »
:horse:
the top layer has many nets and some of them are sensitive nets as you see above.
the second layer is the ground layer. but under these sensitive nets should be ground free!
3rd layer is the power layer.
4th layer is the solder side.

If I want to pour ground polygon in the second layer, this sensitive area will not be ground free! bcoz the nets are in the top layer and I'm in the second layer!

Hi,

I believe that sometime some pictures may be of better help than a lot of words.

Let's assume that you are using a 4 layer board.
The layer stack is set as this:
- TOP layer (signal layer)
- GND layer (plane layer)
- PWR layer (plane layer)
- BOTTOM layer (signal layer)

Signal layers are layers on which you lay traces and polygons and so on. Those are positive layers which means that wherever you see color (polygon pour, fill, traces etc) you will have copper on PCB.
Plane layers are layers meant to serve as a connection for ground nets and power nets. Those layers are negative layers which means that whenever you place "something" (trace, polygon pour, fill etc) in that place occupied by that element, there will be a lack of copper on PCB.

So, what you want is that under the region on top layer occupied by your marked components, on the GND plane, to have a void in the copper, a lack of copper.
This can be obtained by placing a copper fill on the GND plane under that TOP area. But the GND plane being a "plane" and therefore a negative layer, by placing a "copper fill" in the end you get a void in the copper.

Please see the 2D view of such a board in the attached 2D.png
In the 3D view of such a board found in the attached 3D.png, you can sort of see the copper void under the area with the "opamp".

Attached is the Altium 18 PcbDoc file that I've setup and used to get those pictures.

LE: I've added also a picture where I removed all the copper on the PWR plane (by placing a copper fill big as the board) and in the 3D view you can see that the copper is removed by placing that copper fill on GND plane.
« Last Edit: November 25, 2017, 10:06:23 pm by mars01 »
 
The following users thanked this post: xzswq21

Offline xzswq21Topic starter

  • Frequent Contributor
  • **
  • Posts: 295
  • Country: 00
Re: multi-layer PCB design and ground free area in Altium
« Reply #27 on: November 27, 2017, 06:04:39 pm »

LE: I've added also a picture where I removed all the copper on the PWR plane (by placing a copper fill big as the board) and in the 3D view you can see that the copper is removed by placing that copper fill on GND plane.
Dear
you placed a simple solid region under this sensitive area. what's the shape? is it a triangular?
consider you have poured a ground polygon around this sensitive area at the top layer (with 20mil clearance)
can you have a copy of this shape under this area? your solid region is not a copy of the polygon around this area at the top layer.
❤ ❤
 

Offline mars01

  • Contributor
  • Posts: 44
  • Country: ro
Re: multi-layer PCB design and ground free area in Altium
« Reply #28 on: November 27, 2017, 10:59:09 pm »
Now, that your layer stack is made out of 4 signal layers, you can actually draw a polygon pour on your GND layer (the signal layer that you dedicated as GND).

If you want the copper to stay out of that protected area (under your sensitive components) then you simply draw a keep-out solid region on that layer (your GND designated layer) and in Properties you select Restricted for layer: Keep-out layer.

You make sure that this Keep-Out solid region follow closely the perimeter of the protected area. Drawing is done manually.

In Altium Designer 18 you press keys P -> K -> R with your GND designated layer as the active layer.
 
The following users thanked this post: xzswq21


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf