QFN Thermal Via Pitch

Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic

   I am not sure how best to determine the pitch for QFN thermal pads.If I put a via in between the squares of solder paste the pitch is about 1.8mm.
This is using the footprint generated from Footprint Expert.
Some app notes I have read recommend a pitch of 1.0 to 1.5 mm
Is there an IPC spec for this?
I assume there is a way to set the size and number of solder paste squares in Footprint Expert?

Thanks

Author	Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic
jnbrown Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 13 Jan 2020 Status: Offline Points: 40	Post Options Post Reply Quote jnbrown Report Post Thanks(0) Quote Reply Topic: QFN Thermal Via Pitch Posted: 19 May 2021 at 11:57am
	I am not sure how best to determine the pitch for QFN thermal pads. If I put a via in between the squares of solder paste the pitch is about 1.8mm. This is using the footprint generated from Footprint Expert. Some app notes I have read recommend a pitch of 1.0 to 1.5 mm Is there an IPC spec for this? I assume there is a way to set the size and number of solder paste squares in Footprint Expert? Thanks



jnbrown Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 13 Jan 2020 Status: Offline Points: 40	Post Options Post Reply Quote jnbrown Report Post Thanks(0) Quote Reply Posted: 19 May 2021 at 11:59am
	Here is the footprint showing the solder paste squares.

Tom H Members Profile Send Private Message Find Members Posts Add to Buddy List Admin Group Joined: 05 Jan 2012 Location: San Diego, CA Status: Offline Points: 5718	Post Options Post Reply Quote Tom H Report Post Thanks(0) Quote Reply Posted: 19 May 2021 at 12:55pm
	There is an IPC-7093A standard for BTC packages and recommended patterns. There are several controls in V2021 Footprint Expert that allow you to control the paste mask aperture sizes and openings. If you need to control the aperture size and spacing, you must move the QFN footprint to FP Designer and edit the pad stack / Paste Mask layer. In "Tools > Options > Pad Stack Rules > SMD Thermal Tabs > Thermal Tab Minimum Pattern Space" the default setting is 0.20 mm, but you can change the value to control the spacing of the checkerboard pattern. According to the IPC-7093A you can also solder mask define the thermal pad to dam in the paste mask to prevent it from flowing into via holes. This saves PCB fabrication costs because you do not need to plug the via holes. Here is a link to a forum post that has some info on IPC-7093A - IPC-7093A BTC: QFN Solder Mask Defined Thermal Pad - PCB Libraries Forum
	Stay connected - follow us! X - LinkedIn

jnbrown Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 13 Jan 2020 Status: Offline Points: 40	Post Options Post Reply Quote jnbrown Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 8:53am
	Tom, Thanks for the info. When I go to Tools > Options > Pad Stack Rules > SMD Thermal Tabs > Thermal Tab Minimum Pattern Space all of the options are grayed out and I cannot change them. I found the same options on the panel in the lower left and I can change them there. When I change the value Thermal Pad Minimum Pattern Space it has no effect on the solder paste pattern. This pattern has a pitch of about 1.85 mm. I don't see a way to make the pitch smaller. Here is what the footprint looks like in FP Expert: Regarding IPC-7093A and solder mask defined thermal pad, is this something that FP Expert automatically creates or do I have do it manually in Altium? -Joel

Tom H Members Profile Send Private Message Find Members Posts Add to Buddy List Admin Group Joined: 05 Jan 2012 Location: San Diego, CA Status: Offline Points: 5718	Post Options Post Reply Quote Tom H Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 9:02am
	Tools > Options > Internal Defaults cannot be edited. You must File > Save As > your .opt file to edit over 1,000 options. You can create as many option files as you need. Some companies use 10 option files for creating footprints with different rules. There is a "Tools > Options > Pad Stack Rules > Thermal Tab" option for solder mask defining thermal pads. This feature will make the solder mask and paste mask apertures the same size. It dams in the paste mask from flowing and it reduces paste mask voiding.
	Stay connected - follow us! X - LinkedIn

jnbrown Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 13 Jan 2020 Status: Offline Points: 40	Post Options Post Reply Quote jnbrown Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 9:22am
	Ok, I did Save As and now I can edit the options. But changing Thermal Pad Minimum Pattern Space still has no effect on the solder paste pattern.

Tom H Members Profile Send Private Message Find Members Posts Add to Buddy List Admin Group Joined: 05 Jan 2012 Location: San Diego, CA Status: Offline Points: 5718	Post Options Post Reply Quote Tom H Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 9:32am
	Normally, the space between paste mask apertures is greater of 0.50 mm. The default Option setting is 0.20 minimum which means anything greater than that will have no affect. If you select 60% paste mask coverage and enter a 0.50 minimum space, you might not get 60% coverage. Also, most component manufacturers recommend a rectangular shape thermal pad, even though the thermal tab terminal has a 45 degree chamfer. They almost never recommend corner radius on a thermal pad. A rectangle thermal pad is a Flash Aperture for Gerber data. A Chamfered or Radius thermal pad is drawn copper ploy shape and takes long to process. Let me know if you need/want a webcast demo so I can see your screen and help you with your Option settings.
	Stay connected - follow us! X - LinkedIn

jnbrown Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 13 Jan 2020 Status: Offline Points: 40	Post Options Post Reply Quote jnbrown Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 11:54am
	I sent this to our assembler and they are ok with it, so I am going to leave it as is. BTW, I have discussed with them in the past about plugging the vias and they told me that they can assemble it either way but that they get a better solder joint with the vias open. There seems to be some debate about this and no consensus as to whether it is better to leave the vias or plug them.

Tom H Members Profile Send Private Message Find Members Posts Add to Buddy List Admin Group Joined: 05 Jan 2012 Location: San Diego, CA Status: Offline Points: 5718	Post Options Post Reply Quote Tom H Report Post Thanks(0) Quote Reply Posted: 20 May 2021 at 12:15pm
	What happens to the paste mask flow into via holes is that since the vias are connected to the GND planes with direct connections (no thermal reliefs), the solder cools before it goes all the way through the hole and out the back side. Some people are concerned about avoiding problems and they do not assume anything and pay extra to plug the via holes. The 0.20 minimum paste mask gap on the checker board is just to insure that the paste stencil is rugged enough to withstand production. Stencils are expensive and thin webs break. However, the paste stencil web on a 0.40 pin pitch pattern could be smaller than 0.20. We're adding a feature in the Pad Stack Rules Options to allow the user to ensure a 0.20 minimum stencil web on all footprint patterns, but the value is user definable.
	Stay connected - follow us! X - LinkedIn