| Author |
 Topic  |
|
|
shadders
United Kingdom
224 Posts |
 Posted - 16 Dec 2010 : 12:11:34
|
Hi,
Not sure if this can be achieved, but can you exempt pads from the application of thermal relief for copper fills ?.
I have checked on the properties for the Pad - and no selections is stated to exempt from Thermal Relief when copper filling.
Hence - if not possible, is this something that can be provided for in the future ?.
Thanks and Regards,
Richard. |
|
|
tmd63
United Kingdom
18 Posts |
Posted - 19 Dec 2010 : 23:28:00
|
Hi,
It is possible to exemp pads from thermal relief but only for the whole copper pour.
Select the copper pour shape and check the properties. You can select there weather to have thermal relief or not. |
 |
|
|
shadders
United Kingdom
224 Posts |
Posted - 04 Jan 2011 : 12:04:01
|
Hi,
Thanks - I was aware of this - and used it - but some pads have a better connection to a ground plane - example - than others. For those with a limited connection to a ground plane, such as when they are placed in the corner of one, then thermal relief is preferred to be turned off.
In addition, i have PADS which are screw terminals for PCB mounting risers - would prefer these to not have thermal relief.
No response from Number One on whether this is a possible new feature.
Regards,
Richard. |
Edited by - shadders on 04 Jan 2011 12:05:04 |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 22 Feb 2011 : 11:01:31
|
It's a possibility for a new feature. Please send an email to support including your customer ID so it can be formally logged.
Meaanwhile, you can cheat!. Create a different pad style for the pads you want to be exempted. The style wants to be smaller than the actual size by at least the amount of the thermal isolation. After your final pour, edit the pad style to be the size you *really* want. The pad will grow over the gap, and effectively you'll have no thermal break. |
|
|
|
shadders
United Kingdom
224 Posts |
Posted - 23 Feb 2011 : 01:49:09
|
Hi Peter,
Thanks - will give this a try.
Regards,
Richard. |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 23 Feb 2011 : 08:14:38
|
Be careful not to unpour and re-pour after doing this !!! or you will simply end up with thermals on your oversized pads.
If you need to unpour/re-pour you will need to set the pad size back to original and repeat Peters fix as above
Iain |
Edited by - Iain Wilkie on 23 Feb 2011 17:46:35 |
|
|
|
shadders
United Kingdom
224 Posts |
Posted - 23 Feb 2011 : 14:28:13
|
| Thanks Iain. |
|
|
|
Tim_Cyg
United Kingdom
4 Posts |
Posted - 05 May 2011 : 10:43:22
|
Hi,
I have a similar problem to whats described above.
I have a Ground Plane (0V Net) on an inner layer with a through hole pad. On this particular pad (also on 0V Net) - I do not want any thermal break between the pad and the ground plane.
I have tried placing a copper pour area (0V Net) with no thermal break on the ground plane around the pad in question - however this doesn't have the desired result.
Is there any way of achieving this?
Regards,
Tim |
Edited by - Tim_Cyg on 05 May 2011 10:44:32 |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 06 May 2011 : 08:49:41
|
| You need to do basically what is described above. Create the flood with the thermal reliefs. With just one via, it may be easier to right click the pad in question, >properties> increase outer diameter of pad, rather than specify an exception. This way the outer diameter growns over the thermal relief. |
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 02 Apr 2012 : 16:14:47
|
quote:
Originally posted by Peter Johnson
It's a possibility for a new feature. Please send an email to support including your customer ID so it can be formally logged.
Meaanwhile, you can cheat!. Create a different pad style for the pads you want to be exempted. The style wants to be smaller than the actual size by at least the amount of the thermal isolation. After your final pour, edit the pad style to be the size you *really* want. The pad will grow over the gap, and effectively you'll have no thermal break.
Thanks Peter, this works but in my latest project I had 59 pads of 5 different types that I had to set a pad exception for, so it is only practical to use this method for the final copper pour action before going to manufacture.
Possibly the existing pad properties "Plane Connection" selection box could be replicated for Copper pour layers? I would suggest this a 'absolutely must have' feature.
John
John Lawton Electronics |
|
|
|
DavidM
United Kingdom
458 Posts |
Posted - 04 Apr 2012 : 09:16:15
|
On the face of it this does look to be something that ought to be done. I will talk to the team to see if it is feasible to include this in the next release.
David.
|
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 04 Apr 2012 : 10:21:56
|
quote:
Originally posted by DavidM
On the face of it this does look to be something that ought to be done. I will talk to the team to see if it is feasible to include this in the next release.
David.
Thanks David, that's the answer I was hoping for!
John
John Lawton Electronics |
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 15 Jun 2012 : 13:27:56
|
quote:
Originally posted by DavidM
On the face of it this does look to be something that ought to be done. I will talk to the team to see if it is feasible to include this in the next release.
David.
Dear David,
is there any news on this feature in the new release please, the present workaround is very laborious when you have many components, so I consider this feature to be an essential one!
Regards,
John
John Lawton Electronics |
|
|
|
Benno
Netherlands
79 Posts |
Posted - 16 Jun 2012 : 16:13:04
|
Why don't you place a shape around the pad and define that as a keep out for the copper pour?
Still a lot of work, but you only need to do it once.
|
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 16 Jun 2012 : 23:30:07
|
quote:
Originally posted by Benno
Why don't you place a shape around the pad and define that as a keep out for the copper pour?
Still a lot of work, but you only need to do it once.
Because I want the copper pour connection! Typically I want a full 0V net copper pour onto my SMT components pads. I don't want thermals for SMT components as they sometimes look messy and are not needed. However for pth components, thermals are absolutely necessary on copper pour connected pads to enable them to be soldered at all easily.
John Lawton Electronics |
|
|
|
Benno
Netherlands
79 Posts |
Posted - 20 Jun 2012 : 13:03:40
|
| ah OK, now I understand the problem. |
|
|
|
wprov
United Kingdom
15 Posts |
Posted - 25 Jun 2012 : 09:29:13
|
Hi Shadders
Instead of altering the pad as an exception with different diameters you might want to consider the below which would allow as many copper pours as you want without having to keep altering the effected pad(s) each time.
Alternative method (works in V11).
Use a copper pour shape (round or rectangle) and surround the desired pad(s) to over lap any thermal break on same plane as the main copper pour.
Pour copper to pad net with all options unchecked i.e. no thermal relief & no remove.
Pour main copper with normal options re-enabled i.e. thermal relief, remove etc.
End result is a complete copper area with no thermal break on sub copper poured area(s).
You can unpour & re-pour main copper without losing "no thermal relief" on specified pads. Non net pads still get normal clearance to copper pour area as before !.
Note if you move component remember to move sub copper pour and if alter spacing or net guard then re-pour sub copper to ensure matching clearances !.
However might be mute if V6 has requested feature and is about to be released !. But do not count your chickens until hatched !.
|
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 25 Jun 2012 : 09:37:53
|
quote:
Originally posted by wprov
Hi Shadders
Instead of altering the pad as an exception with different diameters you might want to consider the below which would allow as many copper pours as you want without having to keep altering the effected pad(s) each time.
Alternative method (works in V11).
Use a copper pour shape (round or rectangle) and surround the desired pad(s) to over lap any thermal break on same plane as the main copper pour.
Pour copper to pad net with all options unchecked i.e. no thermal relief & no remove.
Pour main copper with normal options re-enabled i.e. thermal relief, remove etc.
End result is a complete copper area with no thermal break on sub copper poured area(s).
You can unpour & re-pour main copper without losing "no thermal relief" on specified pads. Non net pads still get normal clearance to copper pour area as before !.
Note if you move component remember to move sub copper pour and if alter spacing or net guard then re-pour sub copper to ensure matching clearances !.
However might be mute if V6 has requested feature and is about to be released !. But do not count your chickens until hatched !.
Thanks, a clever workaround, wish I'd thought of that. My spies in No. 1 tell me that V16 fixes the issue, but your workaround might still be handy occasionally.
Regards,
John
John Lawton Electronics |
|
|
|
wprov
United Kingdom
15 Posts |
Posted - 25 Jun 2012 : 11:16:55
|
Hi John,
No what is clever is frigging the pcb symbol, pcb file & the gerber output so can get the end result for some thing like TI's TPS6211(n) to pass error check and output correct copper, resist & solder mask !.
Now that is a feat even though EasyPc should be able to do this from day one and has been requested along with others since EasyPC was a little dos program in WIN 3.1 :).
Thanks to the forum members that gave me the idea's to "frig" EasyPc to achieve a work around. Maybe V16 will finally have workable features to upgrade to !.
Sorry a bit off topic !.
|
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 25 Jun 2012 : 12:47:24
|
quote:
Originally posted by wprov
Hi John,
No what is clever is frigging the pcb symbol, pcb file & the gerber output so can get the end result for some thing like TI's TPS6211(n) to pass error check and output correct copper, resist & solder mask !.
Now that is a feat even though EasyPc should be able to do this from day one and has been requested along with others since EasyPC was a little dos program in WIN 3.1 :).
Thanks to the forum members that gave me the idea's to "frig" EasyPc to achieve a work around. Maybe V16 will finally have workable features to upgrade to !.
Sorry a bit off topic !.
What's the problem?
John Lawton Electronics |
|
|
|
wprov
United Kingdom
15 Posts |
Posted - 25 Jun 2012 : 14:06:30
|
Hi John,
“What’s the problem(s)” there fixed it for you !.
Well for mentioned example part you need to make a pcb symbol who has a centre square pad that has 9 holes in it for copper & resist layer but not solder mask layer. In addition it needs 4 smaller square pads for solder mask layer !. Unfortunately you can add resist & solder layers but can not put the pads into those layers (all or top or bottom) !.
Thus work around is to name pads/holes with special names so when add to a pcb you can edit the global pads specially named with various layer exceptions i.e. holes not on copper pad layer (pad to pad errors), large pad on copper & resist only and small square pads on solder mask layer only (pad to pad errors).
Thus add all holes to large pad net (thermal ground), pour sub copper on each layer below large pad (join all holes without thermal break). Solder mask only has reduced square cut outs and resist same size as large pad !.
You need to add solder & resist layers but on output gerber you need to delete the normal resist & solder outputs (will try to output even though make pcb layers same name) so new layers are only correct layers !. All that just to get rid of errors and output desired gerber layers effects!.
Number one needs to fix pcb symbol so can create separate layer specific requirements i.e. make copper & resist & solder specific shapes/pads. Also introduce holes that take on the main pad net when added to pcb file i.e. when add net to main pad holes also take on same net and being a sub part of the main pad does not generate pad to pad error or pad to shape error!.
This opens up many possibilities such as press switch component i.e. copper ½ round pad with shape zig zag line on resist (fingers) and no solder properties. Or the complex pad shape they promised many moons ago by adding a shape to the copper layer and add appropriate shapes to resist and solder mask if needed. Holes would be by adding “holes” !.
Same with pcb file where to add solder to a large area of copper you could add a line shape on the solder mask layer and on the resist layer so the output gerber will have cut outs without mucking around with special layers to subtract/add to certain layers to create the desired end effect i.e. what you see is what you get !.
Old library pcb symbols would still work i.e. if not new format then resist & solder follow old method where copper is same on resist & solder layers.
Others are old text rotate offset effect, sch symbol number & name not flipping when press “F” key (left or right or centre in another menu), flip parts & names shift all over the place (very old bug and suspect where the 3 option came from to move names/numbers back into place rather than fix problem to start with) and other that take too long !.
Well you did ask !.
|
|
|
| |
Topic |
|
Feature Request - Exemption of Thermal Relief