Via sizes increases when custom library com ponent added to PCB

Al schrieb:

HI folks

 

Wonder if you can help. Although I am not a complete newbie to Eagle I

still have limited experience. I have completed double sided designs and

had them made using Gerbers..

 

However I am working on a PCB design uses some new parts which have taken

me into unknown territory.

 

I have created a library part for a QFN component and included links and

vias to take connections automatically to the underside layer. These need

to be very small as follows:

 

Tracks are 0.15 mm and vias are 0.45 mm dia. with 0.25 mm holes

 

Having created the part I then inserted the component in the normal way on

the PCB, however the vias are now much larger! They appear to have grown

and now badly overlap. I even went back to the library part to check the

via sizes which were of course as I had manually set them.

 

Having not gone down this low before for vias I am obviously missing

something important.

 

Can you help me see the error of my ways please

 

regards

Al

The 'vias' you set in the package editor actually are 'pads' and they

have to follow the restring settings in the Design Rules. I suppose

the minimum value for the copper ring arround the drilling is to high.

Try to set it to 0.1mm and also check the value of the precentage.

How Restring settings work can be read there:

  http://www.cadsoftusa.com/faq.htm.en#06012601

HTH

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/faq.htm

Thank you Richard

Changing the Restring settings to 0.1mm worked in that the pads (not vias

anymore) shrank to the correct size, now however I am having problems with

the clearance any suggestions on those settings given the dimensions I

gave?

For the bigger picture I am trying to understand how all of this works,

perhaps you can help me :

My purpose for adding the vias to the package footprint is to eliminate

errors and save work for myself and others in the future. Because of the

high density of this components pads and the difficulty of escaping the

signal wires, I decided to include the vias in the footprint. These

internal vias need to be very specific in dimension and position to use the

part which is why I have such precise position, width, diameter and drill

sizes actually in the package. But if I understand this correctly these

precise details of the package design are effectively overridden when the

component is placed on a board, can you confirm my assumption?

I understand the principles of design rule checking in order to indicate

issues with sizes and proximity etc.. but I don't understand why package

footprints are actually changed when placed on a board, is the 'Restring'

setting a work around to a bug in Eagle until it is fixed as I have not

come across this term before? The problem with the work around you have

suggested is that the part I have added to the library is actually part of

a shared library that will be used by others whom I may not have any

contact with. By designing the package I am  adding to a community library

and thus cannot effect its use later on. In the interests of preventing

everyone that uses this part submitting similar support requests to

yourselves, is there perhaps a better way that I should be adding this

part, as it was meant to make like easier for other folk?

Regards

Al

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Folknology wrote on Wed, 20 January 2010 07:52

Thank you Richard

I understand the principles of design rule checking in order to

indicate issues with sizes and proximity etc.. but I don't understand why

package footprints are actually changed when placed on a board, is the

'Restring' setting a work around to a bug in Eagle until it is fixed as I

have not come across this term before? The problem with the work around

you have suggested is that the part I have added to the library is

actually part of a shared library that will be used by others whom I may

not have any contact with. By designing the package I am  adding to a

community library and thus cannot effect its use later on. In the

interests of preventing everyone that uses this part submitting similar

support requests to yourselves, is there perhaps a better way that I

should be adding this part, as it was meant to make like easier for other

folk?

Hi Al,

First off, as Richard mentioned, you are adding "pads" to the package, not

vias.  Vias can only be instantiated in a PCB.  It's a minor point but if

you use the correct language you'll have an easier time communicating.

Secondly, if you set the diameter of the pad to auto then it will use the

rest-ring settings of the DRC.  But if you set the diameter to some fixed

setting then the rest-ring setting of the PCB DRC won't effect it.  So that

is how you hard code your desired size.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

email:  james@eaglecentral.ca

web: http://www.eaglecentral.ca

Specialising in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Thanks James, I appreciate the clarification.

I will endeavor to use the correct terminology Pad - ' its not a via its a

pad' irrespective of what my pcb supplier insists 'but we call them vias,

the pads are the bits the chip solders to, we make em so we are right,

don't care what you stinking CAD package calls em. etc..'

I manually set the diameter as stated in the precise specifications and

have never used auto for this part for the same reasons. yet the

'rest-ring' setting is having an effect? is this a bug or am I going a

little crazy..

P.S. I have also gone back to double check that the diameter has been set

manually in the library part.

Any ideas?

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

So is there a way to create vias rather than pads in a package?

or can one convert pads into vias?

Or is it that vias are not supported inside packages at all.

In which case the vias would have to be manually added after placement?

Which would be true for BGA packages also yes?

I am obviously a bit confused as I thought adding vias to high density

packages to ease placement was a common industry practice?

Unfortunately PCB manufacturers minimum pad sizes tend to be much higher

than their minimum via sizes.

regards

Al

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

"Al" <al@folknology.com> wrote in message

news:hj72gu$mo5$1@cheetah.cadsoft.de...

Thanks James, I appreciate the clarification.

 

I will endeavor to use the correct terminology Pad - ' its not a via its a

pad' irrespective of what my pcb supplier insists 'but we call them vias,

the pads are the bits the chip solders to, we make em so we are right,

don't care what you stinking CAD package calls em. etc..'

 

I manually set the diameter as stated in the precise specifications and

have never used auto for this part for the same reasons. yet the

'rest-ring' setting is having an effect? is this a bug or am I going a

little crazy..

 

P.S. I have also gone back to double check that the diameter has been set

manually in the library part.

 

Any ideas?

 

http://www.cadsoftusa.com/faq.htm.en#06012601

Restring does resize non-auto sized pads if Eagle deems the pad diameter is

too small.