PCB Design Question: Dealing with various component grids being different

Go To Last Post
12 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

So I've got a question for my fellow PCB designers. How do you folks typically deal with different components on the board that have varying grid sizes?

 

Let me paint a few pictures for you:

 

Notice how in this image I have set the grid size to 0.8mm which matches the QFP and I can get the capacitor to align perfectly to the pin? Well, now the SOIC-16 is also aligned to the same grid but the problem is that component's pin pitch is 1.27mm which means the capacitor won't align to the pin perfectly and looks fairly ugly now.

 

Now take a look at this:

 

Now in this second image I have aligned the SOIC-16 to half of it's 1.27mm grid and left the QFP in it's original location.

 

So just wondering how you guys deal with this? Do you prefer to align your components to a grid that matches its pin pitch or do you use one grid to rule them all?

 

[Edit] Clarification to "aligned the SOIC-16 to it's 1.27mm grid"

My digital portfolio: www.jamisonjerving.com

My game company: www.polygonbyte.com

Last Edited: Wed. Jan 4, 2017 - 04:49 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Lowest common denominator...

 

I typically set to 0.1mm. Personal preference which I am apt to change without even thinking about it.

 

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

valusoft wrote:

Lowest common denominator...

 

I typically set to 0.1mm. Personal preference which I am apt to change without even thinking about it.

 

I guess this would make perfect sense for most (at least the ones I've dealt with) SMD components that typically use metric units so they would align well to a 0.1mm grid but what about through-hole components or even that odd SOIC-16 shift register in my image above that has a grid of 1.27mm (half of the typical through-hole pitch)?

My digital portfolio: www.jamisonjerving.com

My game company: www.polygonbyte.com

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The solution of a fine grid pitch on layout is also what I use. I think that I do use either 0.1mm or 0.2mm, what ever happens to feel good on a given day. The ONLY difference I see is on fine pitch LCC chips (those #%$%* things with the solder surface UNDER the chip). Would also be a problem with BGA, probably. But, not many of us are in that game, I'd guess.

 

Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I repeatedly halve the grid until I can move components to where they look OK.  Usually ends up about 0.15875mm...

I made a menu button to halve/double the grid, and I think it helps keep the larger parts better aligned, compared to picking an arbitrarily small grid...

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Jamison wrote:
How do you folks typically deal with different components on the board that have varying grid sizes?

 

It doesn't matter if components don't "line up" - the electrons don't care. In KiCad it's very easy to change the grid size, so I pick whatever is best for placing the current component  or routing.

Bob. Engineer and trainee Rocket Scientist.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi guy's, it's been a long time, happy new year by the way J

 

What I do first is to place the parts that need to be physically aligned, like displays, led’s, switches, etc, using whatever grid size is needed.

 

After that I use a grid size which corresponds to the PCB manufacture minimum track size, be it 5mil or 6 mil, or whatever they can and still affordable. This makes it easier and faster to manually trace tracks, and also gives a nice looking PCB.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

westfw wrote:
I repeatedly halve the grid until I can move components to where they look OK.

That's a good recommendation!

 

donotdespisethesnake wrote:
It doesn't matter if components don't "line up" - the electrons don't care.

Well, the reasoning for my question is to make my routes look visually appealing. I'd rather not design a board with visual slop.

 

fleemy wrote:
Hi guy's, it's been a long time, happy new year by the way J What I do first is to place the parts that need to be physically aligned, like displays, led’s, switches, etc, using whatever grid size is needed. After that I use a grid size which corresponds to the PCB manufacture minimum track size, be it 5mil or 6 mil, or whatever they can and still affordable. This makes it easier and faster to manually trace tracks, and also gives a nice looking PCB.

Thank you and happy new year to you as well!

 

As to your last comment, this is also what I do. Once I have my components, I stick to a grid size that works well for the specific track size that the manufacturing company can deal with (which is usually 0.5mm) and use that throughout when routing traces. But I tend to also use that same grid for placing components and I've been trying to come up with ways to help align things like passives.

 

I want to thank everybody for the great input!

 

My digital portfolio: www.jamisonjerving.com

My game company: www.polygonbyte.com

Last Edited: Thu. Jan 5, 2017 - 03:38 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Its nice to know that there are individuals with OCD worse than mine!  wink

 

In addition to the "fine grid" approach, some software packages have a "nudge" command, so you can nudge a part L/R or U/D.

It is easy, then, to take the cap that isn't lined up as desired and nudge it left a little bit until it looks lined up when you have zoomed in on that part of the board.

 

Some layout programs also have an "align with this" option.

You identify the reference object, a pin in this case, and the select the target object, the cap in this case, and the software does the alignment for you.

 

Third option, is to line up the components, and not worry about the traces.

When the PCB is completed, having the components lined up is visually more important for a "nice looking board", than having "perfect" traces, without wiggles in them, IMHO.

 

Finally, at the end of the day, others will see the case/box and the display and the knobs and LEDs, etc., and not usually the PCB itself.

So it matters to you, but not to anyone else.

If I was evaluating your work, (potential employer, etc.), I'm more interested in the functionality of the project, and the overall layout, not in whether or not your connecting traces have wiggles in them.

 

For my projects I don't have unlimited time, and the time required for micro-alignment, (pun intended), just isn't worth it.

 

Note that extreme care is often required for RF board work, but that is not the topic under discussion.

 

JC

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

All component placement and routing we do in 1mil (0.0254mm) grid.

That is historically grown.

effectively the grid is there only for your reference.

pick and place machines now a days are getting more and more precision due to components getting finer pitch and smaller.

And if you place components by had it totally is not interesting to have a special grid.

If you got a very busy board you do not want to be getting in trouble with a to coarse grid.

if you have a track of 7 and a grid of 5 and a minimum clearance of 5 then the clearance between tracks will always be 8 so a lot more take 3 of these lines in parallel and you just lost space for 1 line.

As I normally do 'crowbar' designs ( if it fits the board was to big ) I don't want to have things like that.

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

DocJC wrote:

Its nice to know that there are individuals with OCD worse than mine!  wink

 

In addition to the "fine grid" approach, some software packages have a "nudge" command, so you can nudge a part L/R or U/D.

It is easy, then, to take the cap that isn't lined up as desired and nudge it left a little bit until it looks lined up when you have zoomed in on that part of the board.

 

Some layout programs also have an "align with this" option.

You identify the reference object, a pin in this case, and the select the target object, the cap in this case, and the software does the alignment for you.

 

Third option, is to line up the components, and not worry about the traces.

When the PCB is completed, having the components lined up is visually more important for a "nice looking board", than having "perfect" traces, without wiggles in them, IMHO.

 

Finally, at the end of the day, others will see the case/box and the display and the knobs and LEDs, etc., and not usually the PCB itself.

So it matters to you, but not to anyone else.

If I was evaluating your work, (potential employer, etc.), I'm more interested in the functionality of the project, and the overall layout, not in whether or not your connecting traces have wiggles in them.

 

For my projects I don't have unlimited time, and the time required for micro-alignment, (pun intended), just isn't worth it.

 

Note that extreme care is often required for RF board work, but that is not the topic under discussion.

 

JC

 

 

Thanks for the wonderful input, JC! I shall have to see if EagleCAD has a nudge or align to pad. That would be awesome!

I certainly would agree that the components being lined up is visually more appealing than the traces. But I still can't get it out of my head! Eventually I do just have to move on when I can't get it the way I want it.

My digital portfolio: www.jamisonjerving.com

My game company: www.polygonbyte.com

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Almost always:

snap grid: 0.05mm

fine grid: 0.1mm

coarse grid: 1mm (for quick visual measurements)

 

I almost always create footprints by myself. Component  reference point I chose at the intersection of two axis of symmetry if possible. If not, on one axis of symmetry and one edge of the component. Never on a non central pad. If I rotate it, I want it to stay in the same place.

Header with 2.54mm pitch, I place pads at 0, 2.55, 5.5, 7.6, 10.15 and so on. The error is small. This allow me to start or end the trace at the center of the pad. I don't like it to snap to a non grid location.

 

Most of the time the min trace / clearance I use is 0.2mm. I only use smaller one for differential pairs.

 

Me.