Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Removing Polyfill relief for vias in Altium Designer

Status
Not open for further replies.
M

Mattie

Newbie level 4
Newbie level 4
Joined
Feb 22, 2006
Messages
5
Helped
4
Reputation
8
Reaction score
4
Trophy points
1,283
Activity points
1,327
I have used the Polyfill for laying ground planes on both Top and Bottom layers.
Vias are then added to tie the two Gnd planes.
Component pad connecting to Gnd must have thermal reliefs, however I want the Vias to be direct connected.
What is the best way of achieving this?
 

In DRC there is an option for ploygon connect style in that option you can slect the polygon name and via for direct connect.
You can find the excat command for that in tutorials.
 

Yeap Read the tut.
It talks about "Pad class" but I don't seem to be able to get the right class for Vias.
 

Yes as shown in the attached jpg, but in place of "All" you can selct "Is Polygon"
 

If you want pads to still be thermal, you will need to create a second rule (priority order shouldn't matter here) that uses "IsPad" instead of "IsVia" and has the thermal spoke properties you desire.

Not sure if the "IsPoly[gon]" is necessary, it may be implicit in a PolygonConnect rule, but may still be good for clarity/documentation. Just be careful, Altium is inconsistent: plane connection rules use IsPoly, but clearance/back-off rules use InPoly. This probably makes a whole lot of sense to the programmer who implemented the rule system, but not users. You _sometimes_ get a warning if you choose incorrectly.
 

Thanks for the jpg.
I tried something similar and that fixed the Via issue. however the thermal reliefs on all other pads are now very thin.
So I will continue to investigate.
These rules are difficult to comprehend but I must admit their pretty darn powerful.
I'm glad I didn't stay with Client '98!!!
Thanx for the help so far.

Added after 3 hours 13 minutes:

Finally got to try it out again.

Now all is sweet. Added another Polygon rule.
Priority matters.
See the attached screen shots - for future Newbies.
 
TA37 said:
If you want pads to still be thermal, you will need to create a second rule (priority order shouldn't matter here) that uses "IsPad" instead of "IsVia" and has the thermal spoke properties you desire.

Not sure if the "IsPoly[gon]" is necessary, it may be implicit in a PolygonConnect rule, but may still be good for clarity/documentation. Just be careful, Altium is inconsistent: plane connection rules use IsPoly, but clearance/back-off rules use InPoly. This probably makes a whole lot of sense to the programmer who implemented the rule system, but not users. You _sometimes_ get a warning if you choose incorrectly.
Click to expand...



Hi,
this great info I was able to use the above info, I am a newbie to altium, now I need to know how to target a component from the rest of them, with a different thermal relief size.

Thanks to all the pros in altium.
 

Hi,

I just wanted to follow up here, is it possible to mix relief and direct connect vias?
I don't want to set it globally but I would like to have 2 holes in my PCB to be fully connected (for mechanical purpose).
 

For different via rule
Try to change the annular ring size of one via and in design rule try to pass a query like IsVia AND PadXsize All layers = ASMM(XXXX)

- - - Updated - - -

For different via rule
Try to change the annular ring size of one via and in design rule try to pass a query like IsVia AND PadXsize All layers = ASMM(XXXX)
 

anilrock87 said:
For different via rule
Try to change the annular ring size of one via and in design rule try to pass a query like IsVia AND PadXsize All layers = ASMM(XXXX)

- - - Updated - - -

For different via rule
Try to change the annular ring size of one via and in design rule try to pass a query like IsVia AND PadXsize All layers = ASMM(XXXX)
Click to expand...

I figured out 2 things here.
1. Altium is just a state machine the rule can be changed temporarily updating the ring and set it back (as long as the polygons wont be updated they will just remain the same all the time)
2. Set up a Padclass and just add the via to it, that will even survive a polygon update.


The problem is solved now thanks.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top