how to create a pin not ruteable on the top layer? (with altium-protel)

[black_flowers]

i need to keep pins (only the top layer) from routing. Untill now, i've been placing a poligon in order to keepout routing into this poligon, but i'm trying to find out a way to skip routing on the top layer using a property or something like that. Another method i've used is asigning this pad only to bottom layer, but this way it doesn't show the drillhole, and i need it since it's not a smd pad.
I'm using Altium Designer.

thanks.:-D

 

[kevin54]

You should be able to do it with a rule (Design -> Rules -> Routing -> Routing Layers). I haven't tried it but you might just be able to uncheck "Top Layer" under Enabled Layers in the RoutingLayers rule, which I think would disable all routing on the top layer.

 

[black_flowers]

but i don't want to disable all routing in the top layer. I just need to disable routing on those particular pins i cannot reach because they are covered for the body of a commponent. For example in dip encapsulated components i only can reach the bottom layer. I could make that those pins were only on the bottom layer but doing this theres no drillhole on the pin, and i need it. In Cadence there is an option that keeps a pin to be routed in a particular layer but in Altium the only method i found is to draw a keepout region, wich means a lot of work

 

[FvM]

the only method i found is to draw a keepout region, wich means a lot of work

Don't understand your problem with keepouts. If you're using multiple instances, it may be reasonable to include the keepout with the footprint definition.

 

[black_flowers]

my problem with keepouts is that their requires a lot of work since i have to draw a keepout over each pad. If i have a 40 pin package i have to draw 40 keepouts. I cannot draw a keepout over all pins since i don't want to keep the tracks to pass through the coponent: i only keep tracks to be connected to the pins.

What about the property "Electrical Type" which appears in the dialog when you are editting a pad. what happens if i choose "Terminator" type instead of "Load"?

 

[kevin54]

Personally I would put the keepout in the footprint so I would only have to do it once and never again. But it can be done with rules:

1) Create a new Pad Class "TopPadKeepOut" (Design -> Classes -> Pad Classes -> Right-Click -> Add Class -> Right-Click on New Class -> Rename to "TopPadKeepOut")
2) Select any pads you want to have tracks entering only from the bottom, click ">" to make them members of the "TopPadKeepOut" Class
3) Create a Clearance rule to keep all Top Layer nets away from pads in the class "TopPadKeepOut". (Design -> Rules -> Clearance -> Right-Click -> New Rule -> select the new rule "Clearance_1" -> 1st object = "(OnLayer('Top Layer'))" -> 2nd object = "(InPadClass('TopPadKeepOut'))" -> Contraints = "Any Net"

 

[black_flowers]

and how can i do for only definig the pad on the bottom layer, but keeping the drillhole? (If i do that the drillhole disappears)

 

[andre_luis]

black_flowers,

It is very easy to perform at PADS ( Mentor Graphics ).
At Altium, you could put a self-made Pad ( drill + top circle ) created for you, instead regular Pad.

+++

 

[hayat_bilgisi]

Personally I would put the keepout in the footprint so I would only have to do it once and never again. But it can be done with rules:

1) Create a new Pad Class "TopPadKeepOut" (Design -> Classes -> Pad Classes -> Right-Click -> Add Class -> Right-Click on New Class -> Rename to "TopPadKeepOut")
2) Select any pads you want to have tracks entering only from the bottom, click ">" to make them members of the "TopPadKeepOut" Class
3) Create a Clearance rule to keep all Top Layer nets away from pads in the class "TopPadKeepOut". (Design -> Rules -> Clearance -> Right-Click -> New Rule -> select the new rule "Clearance_1" -> 1st object = "(OnLayer('Top Layer'))" -> 2nd object = "(InPadClass('TopPadKeepOut'))" -> Contraints = "Any Net"

i am suffering from the same problem and i thought about the idea above and it seems very logical. But i have no success. Can anybody help us.

Because of component bodies remaining on top layer, for some components i have no possibility to solder from top layer since my prototip boards are non-plated through holes. But i should have the possibility to pass tracks on top layer by vias in order to complete all track connections. I should do this by auto-route strategy because of having many many connections.

i am using altium designer,

Please help,

Thanks a lot.