Offset defined in padstack to match corporate grid
Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: Footprints / Land Patterns
Forum Description: [General or a CAD specific issues / discussions]
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=2726
Printed Date: 21 Dec 2024 at 9:53am
Topic: Offset defined in padstack to match corporate grid
Posted By: StachowJ
Subject: Offset defined in padstack to match corporate grid
Date 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) |
Replies:
Posted By: Tom H
Date 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! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Louis_Guerin
Date 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. |
Posted By: Louis_Guerin
Date Posted: 17 Nov 2020 at 12:20pm
| Smallest placement grid I've use is 0,05mm which is almost halh the line width |
Posted By: Louis_Guerin
Date Posted: 17 Nov 2020 at 12:21pm
half
|
Posted By: StachowJ
Date 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. |
Posted By: cioma
Date Posted: 22 Nov 2020 at 12:26pm
|
Well, if you use 0.001 mm grid then EVERYTHING most likely will be on grid ;) |
Posted By: Tom H
Date 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! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: StachowJ
Date Posted: 22 Nov 2020 at 11:32pm
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 :)
|
cioma wrote:Posted By: Tom H
Date 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! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |