Thermal relief for PowerPAD or MOSFET type components

Making your own components and patterns, organizing and using libraries.
Post Reply
Message
Author
joen
Posts: 9
Joined: 04 Mar 2013, 17:06

Thermal relief for PowerPAD or MOSFET type components

#1 Post by joen » 16 May 2015, 23:14

It doesn't look like DipTrace has any automated via stitching or patterns that have thermal relief. All the parts with power pads are top layer only, at least that is how they come out by default (e.g. patterns QFN-44/8x8x0.65 and TO252-3/10x6.6x2.28). So I copied the TO252-3/10x6.6x2.28 part into my custom library of parts and modified it in this way: 1. I changed pad 3 which is the big guy to "through hole" which makes copper appear on both sides. I made it about 50% larger. Now, there are no vias in the pattern editor so I made a bunch of plated through holes. At least they come plated from my manufacturer. I don't see an option for that. Here is the before part:
TO252-3.png
Here is the frankenpart:
TO252-3STITCHED.png
Will this work? Is it the best way to do this? Are the better ways? Am I totally off on what I am trying to do here? It seems sketchy to me the way I am doing it.

-- 17 May 2015, 22:13 --

I'm starting to think this is not the way to do this. The DRC hates it. In a way it doesn't make sense. But when I try to add vias to the pad in PCB layout it complains there too. Do you do a copper pour around the pad, connect it somehow to the pad and then put the vias in the pour. Or what is the appropriate way to thermally relieve power pads like these in DipTrace?
You do not have the required permissions to view the files attached to this post.

mtripoli
Expert
Posts: 139
Joined: 06 May 2014, 11:56
Contact:

Re: Thermal relief for PowerPAD or MOSFET type components

#2 Post by mtripoli » 20 May 2015, 13:42

I'll tell you how I got around this, but you're not going to like it... I'm not going to do it step by step, a pictures worth...

First, create your pattern in Pattern Editor as shown. The "via" pads need to be outside the main pad as shown. This is because when you go to associate them later if they overlap it won't select the pads correctly:
pads.jpg
Now, open this in Component Editor. Pick the component you want to associate the footprint with. In the footprint preview window, note that you can click on a pad and draw a line to another pad. This associates them to each other:
pads2.jpg
When all pads are associated to each other and the pin it will look like this. Say "OK" to this to close the "Attached Pattern" window. This is important for the next step to update correctly:
pads3.jpg
-- 20 May 2015, 12:43 --

Now the important part. Go back into Pattern Editor and move the "via" pads onto the main pad, making sure to "Save" the updated footprint. Then go back to Component Editor and re-click the footprint from the list. It will update the pad orientation while keeping all previous associations. It will look like this:
pads4.jpg
Say "OK" and "Save" the part. You should have no problems with DRC now...

Good luck!
You do not have the required permissions to view the files attached to this post.

DerekG
Posts: 89
Joined: 18 Mar 2014, 08:06
Location: Norfolk Island

Re: Thermal relief for PowerPAD or MOSFET type components

#3 Post by DerekG » 24 May 2015, 19:12

joen wrote:It doesn't look like DipTrace has any automated via stitching or patterns that have thermal relief.
We are all hoping that the update due in the next 2 or so months will have this feature.

Note that the laws of thermodynamics give the best heat dissipation using vias about 1.0mm apart with 0.3mm holes. It is often wise not to place vias too close to the edge of the central pad, otherwise the MOSFET might "float" to one side when in the infrared reflow oven.

An example is below.

Note that you can also increase the heat dissipation by opening up the bottom solder mask on the tracks/fills leading from the MOSFET. These tracks will then be coated with solder during the wave soldering process (or you can do it by hand).

Note that you can also increase the heat dissipation by opening up the top layer solder mask & "gridding" the solder paste stencil. The "gold" colour shows the "grids" of solder paste that will be layed down.
You do not have the required permissions to view the files attached to this post.
I also sat between Elvis & Bigfoot on the UFO.

User avatar
davenz
Posts: 39
Joined: 01 Apr 2015, 05:55
Location: Christchurch, New Zealand
Contact:

Re: Thermal relief for PowerPAD or MOSFET type components

#4 Post by davenz » 12 Jun 2015, 18:20

I have to say there are some very clever diptrace users out there. Well done those who answered this so thoroughly.
--
All the best,

Dave.

Brent
Posts: 14
Joined: 07 May 2012, 02:59

Re: Thermal relief for PowerPAD or MOSFET type components

#5 Post by Brent » 10 May 2019, 17:09

Have thermal vias been added to DipTrace 3?
Or is this still the best workaround?

Tomg
Expert
Posts: 1336
Joined: 20 Jun 2015, 14:39

Re: Thermal relief for PowerPAD or MOSFET type components

#6 Post by Tomg » 20 May 2019, 15:53

"...Have thermal vias been added to DipTrace 3?..."
No.

"...Or is this still the best workaround?..."
Yes.
Tom

User avatar
KevinA
Posts: 369
Joined: 18 Dec 2015, 15:35

Re: Thermal relief for PowerPAD or MOSFET type components

#7 Post by KevinA » 21 May 2019, 17:52

On a 'onesie' I just use copper pours and Copy Matrix, it's quick.
You do not have the required permissions to view the files attached to this post.

Post Reply