DRC clearance error

RE: DRC clearance error

nav101 — Wed, 06 Nov 2019 09:39:33 GMT

Joern, the minimum is actually 2.6x2.6mm and I did exactly what you said and it got rid of the clearance error.

Thanks

RE: DRC clearance error

autodeskguest — Wed, 06 Nov 2019 09:38:06 GMT

Joern, the minimum is actually 2.6x2.6mm and I did exactly what you said and it got rid of the clearance error.

Thanks

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/284671

RE: DRC clearance error

autodeskguest — Wed, 06 Nov 2019 09:22:04 GMT

Am 05.11.2019 um 21:07 schrieb Rob Pearce:

On 05/11/2019 18:58, Nav Khan wrote:

I am new to this and this is my first design, I was really under the
impression that the librarys available online are accurate. The
manufacturing view of the device shows the central pad so large that
it is touching the other surrounding pads. I should get down to
designing my library...Thanks again

So, first lesson... never trust anybody else's library! This is a rule
that those of us who use Eagle a lot (or, indeed, use any other PCB CAD
software in a professional environment) find ourselves repeating on the
user forum. You cannot trust what you find on the web, to the point that
it's usually quicker just to create the part yourself than search,
download, and verify.

If you're experiencing differences between the library and the board,
this is something of an FAQ. It's down to DRC rules. However, this is
mostly an issue for through-hole components, where the "annular ring"
setting plays havoc with newbies' expectations. In essence, the library
defines the minimum sizes needed for the component, while the DRC rules
define the capabilities of the board house for that project. If the
board house can't achieve the ultra-thin copper ring that the library
defines for a PTH pad, the board gets a fatter one. I wouldn't expect
that to be your problem as it doesn't normally affect SMD pads.

The manufacturing preview may not always be fully accurate. Autodesk
generally say that, where there is a discrepancy, the board editor is
the one to trust. Or you can generate Gerber files and open them in
something like gerbv, which should be definitive.

BTW, the Element14 forum, and the old CadSoft NNTP server it's linked
to, are not the best place for Eagle advice any more. You'd get a better
spread of response (including official support) from the Autodesk forum
at https://forums.autodesk.com/t5/eagle-forum/bd-p/3500

According the data sheet the exposed pad measures 2.5x2.5 mm.

You can check/correct it and maybe the problem is solved.

So, second lesson... never trust anybody else's library! as Rob already

said.

Mit freundlichen Grüßen / With best regards

Joern Paschedag

RE: DRC clearance error

autodeskguest — Tue, 05 Nov 2019 20:07:51 GMT

On 05/11/2019 18:58, Nav Khan wrote:

I am new to this and this is my first design, I was really under the impression that the librarys available online are accurate. The manufacturing view of the device shows the central pad so large that it is touching the other surrounding pads. I should get down to designing my library...Thanks again

So, first lesson... never trust anybody else's library! This is a rule

that those of us who use Eagle a lot (or, indeed, use any other PCB CAD

software in a professional environment) find ourselves repeating on the

user forum. You cannot trust what you find on the web, to the point that

it's usually quicker just to create the part yourself than search,

download, and verify.

If you're experiencing differences between the library and the board,

this is something of an FAQ. It's down to DRC rules. However, this is

mostly an issue for through-hole components, where the "annular ring"

setting plays havoc with newbies' expectations. In essence, the library

defines the minimum sizes needed for the component, while the DRC rules

define the capabilities of the board house for that project. If the

board house can't achieve the ultra-thin copper ring that the library

defines for a PTH pad, the board gets a fatter one. I wouldn't expect

that to be your problem as it doesn't normally affect SMD pads.

The manufacturing preview may not always be fully accurate. Autodesk

generally say that, where there is a discrepancy, the board editor is

the one to trust. Or you can generate Gerber files and open them in

something like gerbv, which should be definitive.

BTW, the Element14 forum, and the old CadSoft NNTP server it's linked

to, are not the best place for Eagle advice any more. You'd get a better

spread of response (including official support) from the Autodesk forum

at https://forums.autodesk.com/t5/eagle-forum/bd-p/3500

RE: DRC clearance error

nav101 — Tue, 05 Nov 2019 18:58:27 GMT

Hi Thanks for the response.

The vias are non issue as I just added them to check if that would help in the clearance. So the clearance issue is still there even without the vias. I am new to this and this is my first design, I was really under the impression that the librarys available online are accurate. The manufacturing view of the device shows the central pad so large that it is touching the other surrounding pads. I should get down to designing my library...Thanks again

RE: DRC clearance error

autodeskguest — Tue, 05 Nov 2019 18:48:23 GMT

On 05/11/2019 17:41, Nav Khan wrote:

I am using a library for MCP73871 battery controller. I tried two different librarys but I get the same clearance error as shown in the picture. This is qfn package where the centre is the exposed pad and is grounded.
Changing DRC clearance does not get rid of the error. Is it a faulty library or am i doing something wrong ... MANY THANKS

There are two separate issues here.

First, the four thermal vias in the centre pad are misaligned such that

one of them is practically touching pin 13. You need to re-centre them.

They're also not being recognised as ground vias, by the look of it,

although the airwires suggest they are correctly named. Which version of

Eagle are you using? I think the rules changed at some point.

Second, you've got pad-to-pad clearance settings in your DRC rules that

don't allow for this footprint. I'm not familiar with the device in

question so I can't say whether the centre pad really needs to be as

large as it is, or whether you need a board house that can manage very

small clearances.

In practice, even if those clearances are OK for manufacture, you may

well need to adjust (or remove and hand-craft) the automatic solder mask

on all the pads of a device like that.