1
\$\begingroup\$

Regarding Mentor PADS Layout software (v9.5)...

I have a large rectangular pad (the tab on a power FET) which is surrounded by a large copper pour (for current and thermal capacity).

When I pour the copper, by default I am given four thin thermal reliefs at the corners of the pad. I want to have more thermal relief spokes in order to promote thermal conductivity into the copper pour and reduce electrical resistance. The FET will be getting warm during use (switching around 4 Amps at various frequencies).

I cannot seem to change the thermal relief settings, how can this be achieved?

I have tried the following... Select the pad and go to Properties...Pad Stack dialog. Then select Pad style: Thermal, click the rectangle icon, then setting the values I want. The preview window shows exactly what I want but selecting OK and exiting the dialog seems to have no effect on the pad's thermals. Going back to that dialog a second time shows that the settings that I asked for ARE remembered but apparently never applied to the actual design.

I have tried unpouring and repouring the copper but it always remains on the default thermal settings (4 at the corners).

How to I make these changes?

\$\endgroup\$

1 Answer 1

2
\$\begingroup\$

DISCLAIMER: I'm using PADS VX.2, so our experiences may differ

Here are the steps I followed:

The pad I'll be changing is the one on the bottom left (the square one with thermal spokes.) Seen here is the original pour, similar to what I would imagine you see on your layout.

enter image description here

I then do what you said, which is go into the Properties>Pad Stacks dialog by right-clicking on the pad I want to change. I then apply the settings I want, again in the same manner you describe:

enter image description here

In this case, the only thing I really changed was going from 4 spokes to 7. Note that this is on an inner layer, but I don't think that will make a difference (though you never quite know with Mentor...) Update: It appears that custom thermals only apply to layers defined as "Split/Mixed" in the layer definition dialog, and that defining outer routing/component layers as Split/Mixed can mess up the CAM output in addition to complicating layout and routing due to the way PADS handles split/mixed layers. Thermals for pours on undefined (i.e., non split/mixed or CAM) layers are handled globally and, as far as I can tell, can't be modified without affecting all plane thermals for those pours. If this isn't acceptable, then the thermals may have to be added manually as copper areas.

Now, I hit OK and it seems the critical difference is at the next dialog:

enter image description here

Without selecting "Keep Attributes", I get the same result as you. If I regenerate the pour without selecting "Keep Attributes", then I end up with the default thermal pattern instead of the custom one I defined in the pad stack dialog. However, if I select "Keep Attributes", then I am able to re-pour the layer (by typing SPO and hitting enter, then re-pouring that plane) and I get the pattern I defined:

enter image description here

\$\endgroup\$
5
  • \$\begingroup\$ That looks right. I'll try this on Monday. The screenshots from your system look to be pretty much the same as on 9.5 (although 9.5 doesn't seem to have an "antipad" feature). \$\endgroup\$
    – user98663
    Oct 28, 2016 at 12:22
  • \$\begingroup\$ Unfortunately it didn't work for me. Perhaps there's a bug in 9.5 but checking that "Keep attributes" box had no effect. I have tried in both ECO mode and normal mode - no luck. :( \$\endgroup\$
    – user98663
    Oct 31, 2016 at 8:24
  • 1
    \$\begingroup\$ Bummer. Is the layer you're pouring defined as split/mixed? According to this answer on the PADS communities, pours on layers not defined as split/mixed won't use user-defined thermals. \$\endgroup\$ Oct 31, 2016 at 11:11
  • \$\begingroup\$ Ah, that might be the problem then. I'm trying to do this on bottom copper which is a normal routing layer. I suppose I'll have to do this the boring way and simply draw copper polygons over the edge of the GND pad. \$\endgroup\$
    – user98663
    Oct 31, 2016 at 12:22
  • \$\begingroup\$ I updated my answer, but unfortunately the answer may be just to do it manually as you say since it doesn't look like Mentor supports this. \$\endgroup\$ Oct 31, 2016 at 12:43

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.