Small Ring Pad - not small enough

On 08.02.2013 12:45, ian . wrote:

Hi,

I'm working on a project with 6.3 that was started in 6.2 - hopefully that won't make a difference.

 

What I want to do is create a pad with a very small ring.

 

In addition, I am trying to do this as part of a library device, so it should be easy.

 

When I draw the package (library editor), I can show Pads any way I like - eg. square pad with drill diam. larger than Pad edge, resulting in a 'Pad' with only the corners attached to a hole.

This is an exaggeration of what I really want, but makes the point.

 

When I Use the device on a .brd, the properties of the Pad are overridden.

 

I've played with Restring values in DRC. I can grow the OD, but can't get it down to the size shown in the Library package.

 

Is there something obvious I'm missing?

 

An alternative approach would be a plated through hole with no ring at all (I'm not sure that's possible).

 

cheers,

 

ian

 

--

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

http://www.element14.com/community/message/69238#69238/l/small-ring-pad--not-small-enough

 

May I add some information about Restring? Hope this helps.....

  How to Define the Pad Diameter?

Since EAGLE version 4.0 the default libraries contain only information

about the drill diameter and the shape of a pad. The diameter value is

set to auto, which is the same as 0, by default.

What does this mean?

The actual diameter will be calculated in the Layout Editor only. The

calculation rule can be found in the Design Rules (menu Edit/Design

Rules…) in the Restring tab. There you are allowed to define different

calculation rules for Top, Bottom, and inner layers.

How is it Calculated?

The percentage, which is related to the drill diameter is used to

calculate the width of the copper ring that is around the drilling.

Default is 25%. A drill diameter of, for example, 0.032 inches results

in a ring width of 0.008 inches.

In the next step EAGLE checks if this value is within the given minimum

and maximum boundaries. If so, the diameter of the pad results for our

example in (2 * 0.008) + 0.032 = 0.048 inches.

Let’s assume the minimum value is set to 0.010 inches. In this case the

previously calculated value of 0.008 inches will be increased in order

to accomplish this criteria to 0.010 inches. The resulting pad diameter

will be 0.052 inches now.

If the calculated value for the restring exceeds the value of the

maximum limit it will be decreased to the maximum tolerated value.

The minimum value represents in principle the Board house’s given

production limits. This is the reason why it is forbidden to exceed the

lower limits.

What Happens if I Define a Diameter in the Package Editor?

If you choose a value for the pad diameter in the Package Editor, EAGLE

calculates again the width of the copper ring by the given percentage as

soon as you add the part to the layout. The calculated value will be

compared to the pre-defined one, resulting from the given diameter in

the library. If the pre-defined value is smaller than the calculated

value or the minimum limit is exceeded, the pad diameter will be increased.

In the case of exceeding the maximum limit, EAGLE will tolerate this.

The pad’s diameter won’t be reduced automatically!

Changing the Design Rules affects the board immediately! Modify the

settings for Restring and click the Apply button and you will see the

result in the layout directly!

Restring settings are valid for all the pads in the layout!

It may happen that the pad diameter shown in the Package Editor or in

the preview of the Device Editor or the Control Panel is not displayed

exactly the same as it is in the Layout Editor because the Design Rules

can be applied in the Layout Editor only!

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

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

Thanks for the reply Richard, I wasn't expecting the reply to only appear in the newsgroup.

From: "Richard Hammerl":

 

May I add some information about Restring? Hope this helps.....

 

 

  How to Define the Pad Diameter?

 

Since EAGLE version 4.0 the default libraries contain only information

about the drill diameter and the shape of a pad. The diameter value is

set to auto, which is the same as 0, by default.

 

What does this mean?

The actual diameter will be calculated in the Layout Editor only. The

calculation rule can be found in the Design Rules (menu Edit/Design

Rules…) in the Restring tab. There you are allowed to define different

calculation rules for Top, Bottom, and inner layers.

 

How is it Calculated?

The percentage, which is related to the drill diameter is used to

calculate the width of the copper ring that is around the drilling.

Default is 25%. A drill diameter of, for example, 0.032 inches results

in a ring width of 0.008 inches.

In the next step EAGLE checks if this value is within the given minimum

and maximum boundaries. If so, the diameter of the pad results for our

example in (2 * 0.008) + 0.032 = 0.048 inches.

Let’s assume the minimum value is set to 0.010 inches. In this case the

previously calculated value of 0.008 inches will be increased in order

to accomplish this criteria to 0.010 inches. The resulting pad diameter

will be 0.052 inches now.

If the calculated value for the restring exceeds the value of the

maximum limit it will be decreased to the maximum tolerated value.

The minimum value represents in principle the Board house’s given

production limits. This is the reason why it is forbidden to exceed the

lower limits.

 

What Happens if I Define a Diameter in the Package Editor?

If you choose a value for the pad diameter in the Package Editor, EAGLE

calculates again the width of the copper ring by the given percentage as

soon as you add the part to the layout. The calculated value will be

compared to the pre-defined one, resulting from the given diameter in

the library. If the pre-defined value is smaller than the calculated

value or the minimum limit is exceeded, the pad diameter will be increased.

In the case of exceeding the maximum limit, EAGLE will tolerate this.

The pad’s diameter won’t be reduced automatically!

 

Changing the Design Rules affects the board immediately! Modify the

settings for Restring and click the Apply button and you will see the

result in the layout directly!

Restring settings are valid for all the pads in the layout!

It may happen that the pad diameter shown in the Package Editor or in

the preview of the Device Editor or the Control Panel is not displayed

exactly the same as it is in the Layout Editor because the Design Rules

can be applied in the Layout Editor only!

 

 

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

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

 

I've emailed my board house to find out their production limit and my final dimensions will be based on this number.

What you describe above is the behaviour I've observed, except that setting the Restring Minimum to 1mil and 1% as well as Sizes - Minimum Width to 1mil.

Unfortunately (for me) this does not result in a small pad.

As a work around. is it possible to to define a plated through hole with no pad? This would allow me to independently dimension the (surface) pad and hole with out it being subject to DRC rules?

ian