Orcad PCB editor - full contact padstack

Hi Everyone,

I'm trying in PCB editor to create a padstack that has full contact to a ground plane. No matter what I try I always get a thermal relief (four spokes) when ideally what I would like is a full contact connection and the hole plated (It is in fact a mounting hole that connects to a copper plane for thermal cooling). I would have thought setting the thermal relief to null and the anti-pad to less than the hole size would make this happen this just does not work.

Any help would be much appreciated.

Ross

In Cadence Allegro PCB (and many other tools), thermal relief usage is a parameter of the shape definition, not of the padstack. In addition, the properties of individual placed pins should be editable. In case of doubt, i would search the PDF or HTML documentation for the respective keywords.

go to shape>global dynamic shape parameters and select thermal relief connects tab. Here you can select to thermal relief contact.

I assume you mean Orcad Layout...
Orcad can be picky about how you setup your board design.
And some settings are rather obscure. Here are some steps to check:

1) Make sure you have defined your BoardOutline obstacle correctly.
Some functions will misbehave otherwise. Your board outline should
be the outermost obstacle, placed on the Global layer, and be of type BoardOutline.

2) Your copper pour obstacle can be any inclosed shape consistent with the
padstack layers you have defined. It should be on the Layer you want to pour,
and be of type CopperPour.

In most cases you will want to assign the pour to a net for DRC. As long as you
are not selecting "seed from object", assigning a net to the pour obstacle does 2 things.
First, it establishes the DRC for the layer, second it allows seeding the pour from
any pin or object on that layer having the same net name.

To turn on copper pouring, go to Options|UserPref and check "enable copper pour" and "use pour for connectivity".

You should see spoke thermal reliefs on your copper pour layer where pins and
pour are on the same net. You usually want this.

But if you want to fill in the spokes for some pins, (like mounting holes), you have
to "FloodPlanesAnPours" for these pins. You can do this in 2 ways:

1) Using the PIN tool, select the pin you want to flood; it will highlite.
While hilited, left-click the SpreadsheetTool and select PadStacks.
The PadStack for the selected pin will come up selected.
Within the spreadsheet, right-click and select Properties.
Here you will see a check box for FloodPlanes/Pours. Check it. Close out back to your board view.

Click the Refresh "!" in the tool bar and your thermal reliefs should be flooded.
Note that this method will flood ALL pins using this padstack that are on the same
net as the copper pour.

2)To be more selective, you can flood only designated pins/padstacks
by making the padstack unique to a component instance. You need to
use the Component Library to do this. In the library, edit the component and
select the pin/padstack as noted above. Check Flood Planes/Pours.
Save component with a new name. Replace the component in your design with this new component.
Be sure to replace only the selected component, not all instances...
Refresh with "!" and you have selective flooding.

One more very subtle note of caution. When creating your copper pour region, be sure to set the
line width for the outline to at least your minimum line width or else you will create strange and
rounded ends on the spokes of your thermal reliefs. You cannot control this artifact by manipulating
the thermal relief settings on the Options tab. If you forget to set this correct, you may find
spokes in your design narrow at the outside to less than minimum design rules!