Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
Search
kicad thermal/ ground stitching vias
|
aurelcristescu
Hello.
I am new to Kicad and I did not find a proper way to resolve these two things: 1) Place thermal vias under a component to transfer the heat to other plane layers (for example connect a QFN with GND pad underneath to an burrier GND plane) 2) Place ground stiching vias to connect TOP and BOTTOM GND layers (like in RF routing). For issue 1 I have tried to place in footprint definition extra pads on the QFN thermal pad (to simulate vias) but they are connecting to GND plane using thermal contours. For issue 2 I have tried to select "Add trace" an then "Place via" and is ok (a GND via will place wherever I like) until I do a UNDO which will remove from all vias GND net association (vias will not have anymore a net associated with them). Do you have any better recommandation for these problems? Thanks in advance. |
|
On 06/06/2012 14:26, aurelcristescu wrote:
Hello. 2) Place ground stiching vias to connect TOP andFirst create two ground zones as required. Then start laying a track at any component pad that is connected to ground. At regular intervals place a via and carry on tracking. The ground track will switch from one layer to the other. Don't return to the start point. Finally fill your zones (I usually just run the DRC to do this). Regards, Robert. -- () Plain text email - safe, readable, inclusive. /\ |
|
Regarding 2) a relevant post that outlines the problem and solution is at http://tech.groups.yahoo.com/group/kicad-users/message/10456. Here is the process I use based on the explanation above: 1. Route the board and define your zones as you always have. 2. Fill the zones as you always have. 3. Select "Add tracks and vias" from the toolbar on the right. 4. Click on an existing pad that¡¯s connected to the zone¡¯s net, drag the pointer a little bit to create a short track, then either (a) right-click and select "Place Via" or (b) type the 'V' shortcut. 5. To add more stitching vias, continue to drag the pointer and type 'V' where you want to drop vias (or right-click and select "Place Via"). 6. When you are done placing vias, hit the 'End' key on your keyboard (or right click and select "End Track"). You can repeat this as many times as you want to create different clusters of stitches. When you refill zones, the vias will retain the connectivity information and work as expected. -Mithat
|
|
this is exactly what I do, I find it kinda annoying... there should be better way. i tried just stitching some vias without using trace and that was a bad idea. actually the idea was good but PCBNew didn't work as expected - vias placed this way didn't get the net assigned. as a result PCB was fine but if one had to reflow zone for example or just run DRC, all those vias would become orphans. From: Robert To: kicad-users@... Sent: Wednesday, June 6, 2012 9:51:32 AM Subject: Re: [kicad-users] kicad thermal/ ground stitching vias
?
On 06/06/2012 14:26, aurelcristescu wrote: > Hello. > > I am new to Kicad and I did not find a proper way to resolve these > two things: > > 1) Place thermal vias under a component to transfer the heat to other > plane layers (for example connect a QFN with GND pad underneath to an > burrier GND plane) > 2) Place ground stiching vias to connect TOP and > BOTTOM GND layers (like in RF routing). First create two ground zones as required. Then start laying a track at any component pad that is connected to ground. At regular intervals place a via and carry on tracking. The ground track will switch from one layer to the other. Don't return to the start point. Finally fill your zones (I usually just run the DRC to do this). Regards, Robert. -- () Plain text email - safe, readable, inclusive. /\ |
|
Aurel Cristescu
I?think I got the idea. Both #1 and #2 are working ok (they are not loosing their net - GND -when UNDO is pressed or file is reopened)?IF they have a trace connection to a netlist defined pin.
?
#1 See thermal_vias_...jpg
Thermal vias were added like that: add trace from pin 20 (GND) to center of pin 33 and place via. Then each via was moved on desired position and trace was preserved (not deleted).
If you reopen BRD or make an UNDO cycle the vias will preserve GND net connectivity.
#2 See gnd_pane.... jpg
As advised by Robert
?
Thanks a lot for help
From: Ivica Kvasina
To: "kicad-users@..." Sent: Thursday, June 7, 2012 4:38 AM Subject: Re: [kicad-users] kicad thermal/ ground stitching vias ?
this is exactly what I do, I find it kinda annoying... there should be better way.
i tried just stitching some vias without using trace and that was a bad idea. actually the idea was good but PCBNew didn't work as expected - vias placed this way didn't get the net assigned. as a result PCB was fine but if one had to reflow zone for example or just run DRC, all those vias would become orphans.
From: Robert To: kicad-users@... Sent: Wednesday, June 6, 2012 9:51:32 AM Subject: Re: [kicad-users] kicad thermal/ ground stitching vias ?
On 06/06/2012 14:26, aurelcristescu wrote: > Hello. > > I am new to Kicad and I did not find a proper way to resolve these > two things: > > 1) Place thermal vias under a component to transfer the heat to other > plane layers (for example connect a QFN with GND pad underneath to an > burrier GND plane) http://tech.groups.yahoo.com/group/kicad-users/files/QFN_MLF/ http://tech.groups.yahoo.com/group/kicad-users/files/IPC%20Modules/ > 2) Place ground stiching vias to connect TOP and > BOTTOM GND layers (like in RF routing). First create two ground zones as required. Then start laying a track at any component pad that is connected to ground. At regular intervals place a via and carry on tracking. The ground track will switch from one layer to the other. Don't return to the start point. Finally fill your zones (I usually just run the DRC to do this). Regards, Robert. -- () Plain text email - safe, readable, inclusive. /\ http://www.asciiribbon.org/ |
to navigate to use esc to dismiss