Answer to your questioin - Yes, you can define 'copper pour' shapes on the solder mask. Think of them as solder mask pours.
When I've done this in the past I don't place vias under the part. I define additional pads (and pins on the schematic) so that they are defined with the part. I define a copper shape for the thermal pad and associate it to an appropriate pad. Once the pins are connected together on the schematic there are no design errors because the thermal shape lays over all the other pads. An example (without tenting) is attached.
I believe you'll have to update your Gerber generation to include shapes on the soldermask layer. There may have been a few other steps in there too.
How did you get an image to show up in the middle of your post?!? I like that!
thermalpad.bmp 161.8 KB
Thanks for the response. I had seen your technique with the vias in my hunting. Your comment about the associated copper got me headed in a direction toward a good result.
I chose to add a terminal in place of one of the dots I created on the paste mask layer (stencil). Then, instead of associating copper to it, I just added copper in the shape of the actual thermal pad(not associated). This pad only contributes a small dot right where I want it to be on both the solder mask and paste mask layers. On the solder mask layer, I use the same pattern shown in my original post (green area), and it swallows the dot from the terminal. On the paste mask layer, I also use the same pattern shown in my original post (blue dots), and the dot from the terminal just shows up in the same spot as the dot on the paste mask layer.
I am not going to include the vias on the decal, since there may be cases where they are not wanted.
So the process looks like this:
1) Create the part footprint, but make the terminal for the thermal pad a small dot (or other shape) where one of the stencil openings is going to be.
2) In the decal editor, arrange "copper" on the solder mask layer to create an opening for the pad that has the "tents" where I plan to place vias
3) In the decal editor, arrange "copper" dots on the paste mask layer to create the openings for the solder paste
4) Once the part is placed on the board, decide whether or not to add vias to the other planes for heat sinking
5) Use the cam tool to show the copper shapes on the solder mask and paste mask output
In getting to this point, I first used the method of associating the copper with the terminal. In that case, I had to use the advanced setting for "pads with associated copper" in the cam tool to keep the associated copper from showing up on my silkscreen and paste mask layers. Unfortunately, turning off the associated copper affects other parts that have associated copper (makes it so the associated copper does not open in the mask for parts that you would want it to).
When we create our cam output for solder mask and paste mask, we use the pads on the top or bottom layer as the starting point. The bottom line is that it appears the only way to have full control of the solder mask layer would be to create a copy of each pad on the solder mask and paste mask layer for each component decal when it is created. This way you can customize what it looks like without relying on the copper shapes on the top/bottom layers.
BTW, I just used the little camera icon to add the image in-line. They may have a file size limit for this feature that prevented your image from being shown in-line.
"I am not going to include the vias on the decal, since there may be cases where they are not wanted."
That sounds error prone. Another designer may see the tents and assume that the vias are already in place. I recommend adding the vias (component pads) to your standard part. if someone needs to delete them for a specific board they can make those changes on the PCB. If they later update the footprint from the library they'll have issues but that will be easy to clean up.
Thanks for the tip on the camera!
all your hard work may be for naught
paste masks are seldom used as they come from CAM output without being modified
one reason many simply give a 1:1 of the smd
and let the manf eng and stencil maker tweak it to to what their experience tells them.
even then they often go thru 2-3 iterations before they get it right
adding the vias to the decal is a good idea if you seldom have comps on both sides of the board
but if you often do, it may be better to leave them out and add manually since you don't want to tie your hands of available real estate on the back side of the board for placement
I used to think that too until I had an assembly house put my job on hold because they didn't like my solder paste layer. This was a low volume house so they wanted all the 'engineering' done before they got the job. i agree that almost all higher volume houses will tweak it to their process.
Yup, unless you're dealing with a low-volume "we want everything done up front" shop, let the assembler worry about the paste. I used to work for a company that does assembly, they liked 80% coverage for the solderpaste.
And they liked the vias untented under the part. Actually, they liked the soldermask opening to be 1:1 (or slightly oversized) to the GND slug pad.
The nice thing about those "we want everything done up front" shops, they usually have very specific guidelines for how they want past and mask handled.
Yup, let the assembler worry about the paste. I used to work for a company that does assembly, they liked 80% coverage for the solderpaste.
Good to know.
In my case, I am dealing with low volume and a local CM. All the heavy lifting is done by us .
My wife wants to figure out a way to do Lego mini-figure costumes for our boys this Halloween. Is that a picture of a costume you made? If so, would you mind sharing some construction tips?
I should have said: "They liked 1:1 soldermask openings, then we would modify as specified by our component engineer. They liked about an 80% coverage for the solderpaste."