Atium Designer Question

[edonor]

altium net tie

Does someone know how it is possible to trace separated planes of GND that later join in a concrete point?
How is it possible to do automatically in Atium Designer?

 

[House_Cat]

altium designer net tie

If you hold the Control key while clicking on one of the net connections, all of the portions of the board to which that net is connected will be highlighted, and the rest of the board will be masked.

You can also use the PCB Panel. Go to the top of the panel, select Nets, click on "All Nets". Wait for Altium Designer to sort the nets, then click on the name of the net in the center part of the panel. All of the chosen net will be highlighted, and the rest of the board will be masked. All of the objects in the chosen net will appear in the bottom part of the panel.

If you use Edit>Select>Net (hotkey SN) to select a single connection in a net, all of the connections in that net will be selected.

 

[artem]

net tie altium

Ctr-H changes cursor to permanent copper highlight mode as clicking to portion of track will highlight entire net.

 

[House_Cat]

where do i find the altium net tie

Ctr-H changes cursor to permanent copper highlight mode as clicking to portion of track will highlight entire net.

That's true, artem - however, if you use Ctrl-H and click on a via connected to a plane, only the single via and the direct connections to it will highlight - other connections to the net elsewhere on the plane will not. If you use "SN", ALL of the connections on that net will be selected across the entire board.

 

[artem]

altium net tie component

May be i am wrong , but i have just checked that on v 6.6 and clicked to via after ctr-h - the entire net was selected. Board is 2 layer .

 

[House_Cat]

altium net ties

May be i am wrong , but i have just checked that on v 6.6 and clicked to via after ctr-h - the entire net was selected. Board is 2 layer .

If your board is only two layers, it does not have plane layers. Ctrl-H is the shortcut for "select connected copper" - it has nothing to do with net definitions. You are apparently seeing a copper connection through a polygon on your two layer board. With a true plane layer, Ctrl-H will NOT select all of the net connected to the plane. Remember that plane layers in Protel/Altium Designer are negative layer representations - there's no copper representation to complete the connectivity for the Ctrl-H command.

I suggest you try the functions on one of the 4 layer example boards packaged with Altium Designer to see how the various functions work.

 

[edonor]

net ties in altium

Thanks for your answers, but I'm asking for other question.

I've an schematic with 2 grounds (GND and AGND) and I want to route in an independent way, two different nets. Finally I will joint both in one point.

How to do this without 0 ohm resistors?

Thanks.

 

[House_Cat]

altium nettie

You need to create a special component called a "net tie" on both your schematic and your PCB. A "net tie" allows you to connect two different nets without generating a DRC error.

A "net tie" on the schematic side is just two back-to-back pins with the property defined as a net tie. See page 93-94 in "TR0111 Schematic Editor and Object Reference.pdf" for a description.

On the PCB side, the net tie can be whatever you need. I generally use a couple of single layer pads joined by a track. However, you could use thru-hole pads joined by a track. You define your component as a net tie in the component properties dialog under "type".

 

[edonor]

altium component type net tie

Thanks House_Cat

 

[Siliconray]

altium add net tie

Hi,

When I use Situs-auto router(Altium designer). I always get a lot of

Short-Circuit Constraint (Allowed=No) (All),(All)

What should I change to get less Short-Circuit Constraint. I use bga-footprint and under bga I get short-circuit.

r,S