PCB Libraries Forum Homepage
Forum Home Forum Home > Libraries > Footprints / Land Patterns
  New Posts New Posts RSS Feed - Offset defined in padstack to match corporate grid
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

Offset defined in padstack to match corporate grid
 Post Reply Post Reply
Author
Message
  Topic Search Topic Search  Topic Options Topic Options
StachowJ View Drop Down
New User
New User


Joined: 17 Oct 2018
Status: Offline
Points: 7 		Post Options Post Options   Thanks (0) Thanks(0)   Quote StachowJ Quote  Post ReplyReply Direct Link To This Post Topic: Offset defined in padstack to match corporate grid
    Posted: 17 Nov 2020 at 5:32am

I'm a librarian in my company. We are introducing new EDA on global level. Some features are still unknown for us (introducers) and have to be discovered and get familiar with.

Today I've got a request to implement an offset in padstacks so that pads in cells match the project grid. We will define particular grid in which PCB should be designed (placement, routing, vias, TPs...).

One of layout engineers complained that a trace between two pads of two components doesn't route straight. He would like to have an offset in pad to match global grid.

I said that we can implement round-offs (for placement and size) but in general it won't solve his problem. 

Is this a common approach (to add offset for origin of pad/padstack to have traces (all segments) in project grid)?

(I hope I described it well enough, if not I could try to explain it better)
Back to Top
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 17 Nov 2020 at 9:25am
Using Library Expert V2020.03, you can easily do this in - 
"Preferences > Terminals > Select any Terminal > Settings > Pad Place Round-off and Pad Size Round-off"

Library Expert will prompt you if you want to apply this new setting to All Terminals. Select "Yes". 
Stay connected - follow us! X - LinkedIn
Back to Top
Louis_Guerin View Drop Down
Active User
Active User
Avatar

Joined: 29 Jan 2013
Location: Quebec
Status: Offline
Points: 24 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Louis_Guerin Quote  Post ReplyReply Direct Link To This Post Posted: 17 Nov 2020 at 12:18pm
Hi,
Although you can do it, like on connectors, offsetting pad from hole location to ease paste in pad for reflow, it's not, IMHO, something to do just for routing aesthetics on CAD tool.
After doing layout for over 30 years I've never done nor see components pads offset just to have straight lines. It was always for other purposes.
You will always got some placement issue due to density where preferred grid placement will have to be overridden.
Most of today's layout tool are grid less because of such components terminations and placement density. 
Smallest placement grid I've use is 0,05mm which is almost twice the line width you will use on a board without having to pay for a premium from most pcb fab house and even then, line width can vary due to fab process in a way that on board you won't see it if it's not straight.
Then are also the possibility to do fanout where you could go on a 0,5mm grid for component as small as 0402 (1005 metric) or go Via In PAD, when needed or bring your trace to a place on pad where the line will be straight and finish it to the pads snap point.

Unless you have someone to validate component attachment integrity on board from what it's define on spec sheets or calculators I'm not recommending it.



Back to Top
Louis_Guerin View Drop Down
Active User
Active User
Avatar

Joined: 29 Jan 2013
Location: Quebec
Status: Offline
Points: 24 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Louis_Guerin Quote  Post ReplyReply Direct Link To This Post Posted: 17 Nov 2020 at 12:20pm
Smallest placement grid I've use is 0,05mm which is almost halh the line width
Back to Top
Louis_Guerin View Drop Down
Active User
Active User
Avatar

Joined: 29 Jan 2013
Location: Quebec
Status: Offline
Points: 24 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Louis_Guerin Quote  Post ReplyReply Direct Link To This Post Posted: 17 Nov 2020 at 12:21pm
halfCensored
Back to Top
StachowJ View Drop Down
New User
New User


Joined: 17 Oct 2018
Status: Offline
Points: 7 		Post Options Post Options   Thanks (0) Thanks(0)   Quote StachowJ Quote  Post ReplyReply Direct Link To This Post Posted: 18 Nov 2020 at 12:50am
Hi Both,
thanks for your answers.
@Tom I know that I can apply the round-offs, we will do that. My question was more about moving pad's origin so that pad snaps into the grid of whole pcb design. My colleague doesn't like these little segment insite pad when routing. So everything comes to the aesthetics :) I think @Louis understood my question :) For sure some parts require offsets on pads, that's clear. Request was more about common packages (0805, 0402, SOT23...) I will try to convince to use round-offs only.
Back to Top
cioma View Drop Down
Advanced User
Advanced User


Joined: 17 Jul 2012
Status: Offline
Points: 149 		Post Options Post Options   Thanks (1) Thanks(1)   Quote cioma Quote  Post ReplyReply Direct Link To This Post Posted: 22 Nov 2020 at 12:26pm
Well, if you use 0.001 mm grid then EVERYTHING most likely will be on grid ;)
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 22 Nov 2020 at 2:32pm
A 1 um grid might be popular in the future. 

Right now, a 10 um grid system is OK for pad stack size, snap grid and rounding. 

Note: V2021 Footprint Expert will support a 0.000001 mm grid to eliminate rounding issues when converting back and forth from metric to imperial units. But the end user sets the minimum and maximum unit's. 
Example: the default metric unit setting is minimum 2 places, maximum 3 places but the user can change that to up to 6 places for both min/max.
Stay connected - follow us! X - LinkedIn
Back to Top
StachowJ View Drop Down
New User
New User


Joined: 17 Oct 2018
Status: Offline
Points: 7 		Post Options Post Options   Thanks (0) Thanks(0)   Quote StachowJ Quote  Post ReplyReply Direct Link To This Post Posted: 22 Nov 2020 at 11:32pm
Originally posted by cioma cioma wrote:

Well, if you use 0.001 mm grid then EVERYTHING most likely will be on grid ;)
Then grid makes no sense somehow :)
Anyway thanks for you answers. We came to the point in the company that everything will be incremended by 0.05 mm step, all values will be rounded to that. Should be fine :)
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 24 Jan 2022 at 10:17am
Ideally all objects in a PCB layout can be in 0.05 mm increments. 

SMD and PTH Pad Sizes, Trace Widths, Via Sizes, Hole Sizes, Copper Pour Shapes in 0.05 increments but part placement grid should be in increments of 0.10. 

That's a grid system that works well with medium to large footprints. But if your PCB design is loaded with microminiature components like a Cell Phone board, you must us a 0.01 grid system. 

But we're headed in the 1 micrometer (0.001 grid system) direction by 2030 as microminiature technology will be the norm. 

I can't see far enough into the future that will require going beyond a 0.001 grid system. 
Stay connected - follow us! X - LinkedIn
Back to Top
 Post Reply Post Reply

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.250 seconds.