How do you make vias in the ground pad of an IC without making them into pads. Normally this isn't a problem form me but i'm doing one that has 41 vias! Its hard to fit that many on the corresponding schematic symbol.
thanks,
Dave Grundy
making vias in ground pad of IC
Re: making vias in ground pad of IC
"...How do you make vias in the ground pad of an IC without making them into pads..."
I'm assuming you are referring to the application of thermal vias to a pattern, for which DipTrace has no dedicated solution. Here are a couple of thermal via work-arounds that were discussed a while back - https://www.diptrace.com/forum/viewtopi ... =5&t=10445
"...Normally this isn't a problem form me but i'm doing one that has 41 vias! Its hard to fit that many on the corresponding schematic symbol..."
I wasn't aware that a schematic representation for thermal vias was necessary. I always thought thermal vias only needed to be created in the Pattern Editor (have to use pads here) or the PCB Editor (you can use vias here). When creating the pattern in the Pattern Editor make sure to connect all of those so-called "vias" (pads in this case) to the ground pad. When adding vias in the PCB Editor, assign all of them to the same net as the ground pad.
I'm assuming you are referring to the application of thermal vias to a pattern, for which DipTrace has no dedicated solution. Here are a couple of thermal via work-arounds that were discussed a while back - https://www.diptrace.com/forum/viewtopi ... =5&t=10445
"...Normally this isn't a problem form me but i'm doing one that has 41 vias! Its hard to fit that many on the corresponding schematic symbol..."
I wasn't aware that a schematic representation for thermal vias was necessary. I always thought thermal vias only needed to be created in the Pattern Editor (have to use pads here) or the PCB Editor (you can use vias here). When creating the pattern in the Pattern Editor make sure to connect all of those so-called "vias" (pads in this case) to the ground pad. When adding vias in the PCB Editor, assign all of them to the same net as the ground pad.
Tom
-
dhgrundysr
- Posts: 8
- Joined: 08 Mar 2016, 15:49
Re: making vias in ground pad of IC
Hi Tom,
thanks for the reply
so i guess i can just not enter these additional pads in the schematic symbol, and ignore the warning message.
thanks,
Dave
thanks for the reply
so i guess i can just not enter these additional pads in the schematic symbol, and ignore the warning message.
thanks,
Dave
Re: making vias in ground pad of IC
I found that by
1)making the SMD ground / thermal pads that are a part of the IC, then placing the THT pads in those SMD pads in the correct positions and as any as are needed.
2) Then assigning the SMD pads the correct pad numbers, followed by assigning the THT pads that are placed in the SMD pad the same number as the SMD pad.
3) When assigning the pad numbers use the following format: (pad number; @ symbol) ie.. 20@
I would add photographs but I can't seem to cut and paste them here.
1)making the SMD ground / thermal pads that are a part of the IC, then placing the THT pads in those SMD pads in the correct positions and as any as are needed.
2) Then assigning the SMD pads the correct pad numbers, followed by assigning the THT pads that are placed in the SMD pad the same number as the SMD pad.
3) When assigning the pad numbers use the following format: (pad number; @ symbol) ie.. 20@
I would add photographs but I can't seem to cut and paste them here.
Re: making vias in ground pad of IC
Why would you want the thermal vias to show in the schematic? Assume a 14 pin package with a big thermal pad: What I've done in Altium and other packages is to add one more pin which is called Thermal, which has a number higher than the highest real pin, (pin 15 on a 14 pin package) and create the pad in the footprint library corresponding to that pin number. In the schematic then tie pin 15 to ground, and that's all I need. So the grounded heatsink pin appears in the schematic lest you forget, but it's not a whole bunch of pins, just one.