Author Message
 Post subject: How to change a through hole inner layer pattern
PostPosted: 04 Jul 2016, 05:45 
Offline

Joined: 31 May 2016, 10:04
Posts: 3
Hi all,

got a problem with through hole. I have a DIP device which I create in pattern editor with a inner hole 0.8mm and outer pad diameter 1.6mm. How do I make the through hole with inner layer with a 0.8mm hole and outer pad diameter 1mm ?
Could anyone help? Thanks a lot.


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 07 Jul 2016, 19:25 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 944
alextien wrote:
"...How do I make the through hole with inner layer with a 0.8mm hole and outer pad diameter 1mm?..."
To my knowledge, this is not possible in DipTrace. If you don't need a connection from that pad to the inner layer in question, you can eliminate the inner layer pad completely. If this is okay with you, here is how to do it...
1) Bring up/display the desired inner layer (press hotkey 1, 2, 3, or whatever number coincides with that layer).
2) Right-click on the desired pad.
3) In the pop-up menu, select Hide Pad Ring in Layer.

Note: Clearance voids for copper pours on other nets will be the same size for hidden pads as they are for the normal pad. And if the pad is on the same net as the copper pour, the copper pour clearance will be very small, almost touching; but it still will not connect.


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

_________________
Tom


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 10 Jul 2016, 05:47 
Offline

Joined: 31 May 2016, 10:04
Posts: 3
Tomg wrote:
alextien wrote:
"...How do I make the through hole with inner layer with a 0.8mm hole and outer pad diameter 1mm?..."
To my knowledge, this is not possible in DipTrace. If you don't need a connection from that pad to the inner layer in question, you can eliminate the inner layer pad completely. If this is okay with you, here is how to do it...
1) Bring up/display the desired inner layer (press hotkey 1, 2, 3, or whatever number coincides with that layer).
2) Right-click on the desired pad.
3) In the pop-up menu, select Hide Pad Ring in Layer.

Note: Clearance voids for copper pours on other nets will be the same size for hidden pads as they are for the normal pad. And if the pad is on the same net as the copper pour, the copper pour clearance will be very small, almost touching; but it still will not connect.


Thanks a lot for your answer.
The problem is I still need to have connection for the inner pad.
Could I just simply hide pad ring in layer and put my desired pad over the pin?


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 10 Jul 2016, 07:01 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 944
alextien wrote:
"...Could I just simply hide pad ring in layer and put my desired pad over the pin?..."
Yes, but even after making the necessary Net connection between the two different pads, the DRC would still flag it as a pad-to-pad clearance error. It is also possible that the PCB manufacturer might be concerned with two drill holes being in the same place and halt production until they talk to you about it. In that case it would be prudent to let them know about the extra pad/hole in advance to see how they would prefer to handle it.

alextien wrote:
"...I still need to have connection for the inner pad..."
Since you desire an electrical connection anyway, I would suggest changing the entire pad stack to the smaller ring size.

Whatever choice you make, don't make the ring size too small or you may run into hole breakout problems due to manufacturing limitations.

-- 10 Jul 2016, 07:36 --

Another alternative would be to...
1) Hide the inner-layer pad.
2) Create a small, circular, 1mm diameter, filled signal/plane shape on the same inner layer.
3) Assign the new shape to the same Net as the pad.
4) Choose the smallest grid size available (.003mm?), select/highlight the shape and move it (use arrow keys) into a position that is concentric with the pad.

This would avoid the extra drill hole and eliminate any DRC clearance errors.

-- 10 Jul 2016, 08:58 --

Upon further investigation I've discovered that connecting a trace to the last suggested work-around (circular shape on same Net as pad) will result in a "Connection without a pad ring" DRC violation. I guess it all comes down to which error you are most comfortable ignoring.


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

_________________
Tom


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 11 Jul 2016, 05:30 
Offline

Joined: 31 May 2016, 10:04
Posts: 3
Quote:
Upon further investigation I've discovered that connecting a trace to the last suggested work-around (circular shape on same Net as pad) will result in a "Connection without a pad ring" DRC violation. I guess it all comes down to which error you are most comfortable ignoring.


Thanks a lot for your answer, it really help.


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 12 Jul 2016, 02:08 
Offline
Technical Support

Joined: 14 Jun 2010, 06:43
Posts: 2762
If you change internal layer type to plane you can specify custom pad ring on the layer. It means all through-hole pads will have round shape and all pad diameters will be equal pad hole plus custom pad ring on the layer.


Top
 Profile  
 
 Post subject: Re: How to change a through hole inner layer pattern
PostPosted: 13 Jul 2016, 15:59 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 944
Alex wrote:
If you change internal layer type to plane you can specify custom pad ring on the layer. It means all through-hole pads will have round shape and all pad diameters will be equal pad hole plus custom pad ring on the layer.
Is this what you are referring to?...


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

_________________
Tom


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 7 posts ] 

All times are UTC - 5 hours [ DST ]


Who is online

Users browsing this forum: No registered users and 5 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group