Making pads with oval holes

I don't know how it got changes, but that was supposed to be Eagle

4.16... not 6.16... I wish I had version 6 available...

--

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

http://www.element14.com/community/message/88377#88377

On 9/5/2013 10:06 AM, Ernie Thomas wrote:

I don't know how it got changes, but that was supposed to be Eagle

4.16... not 6.16... I wish I had version 6 available...

 

--

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

http://www.element14.com/community/message/88377#88377

 

Hi Ernie,

It is possible, I've attached a short procedure for that.

hth,

Jorge Garcia

On 9/5/2013 10:06 AM, Ernie Thomas wrote:

I don't know how it got changes, but that was supposed to be Eagle

4.16... not 6.16... I wish I had version 6 available...

 

--

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

http://www.element14.com/community/message/88377#88377

 

Hi Ernie,

It is possible, I've attached a short procedure for that.

hth,

Jorge Garcia

Jorge Garcia wrote on Tue, 10 September 2013 15:40

On 9/5/2013 10:06 AM, Ernie Thomas wrote:

I don't know how it got changes, but that was supposed to be Eagle

4.16... not 6.16... I wish I had version 6 available...

 

--

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

http://www.element14.com/community/message/88377#88377

 

 

Hi Ernie,

 

It is possible, I've attached a short procedure for that.

 

hth,

Jorge Garcia

 

In order to make slots follow this procedure:

 

1. For the moment ignore the drill hole worry only about getting the

overall pad shape close to the size you need.

2. Once the pad is approximately the correct size you can draw in the

opening using the WIRE command on a non-copper layer such as milling

Layer 46.

3. When you go to generate the gerbers you will generate a separate

gerber file containing only layer 46. You will tell your board house that

the info on that gerber needs to be milled from the board. Let me know if

there's anything else I can do for you.

It's not that easy Jorge.  If you do that, then internal power planes will

not have cutouts for the milled out area.  As a result, your pad will be

connected to all the internal layers when you have your board manufactured.

That means all our internal layers will be shorted together too.  EAGLE

doesn't handle this well and we need much better way to handle these.

Right now, the best workaround I have is to add the wires added on layer 46

to layer 20 (dimension) as well.  The copper pouring will honour that and

create openings on internal power planes.  However, this won't work if you

actually do want the pad to connect to those internal pads.  So currently,

there is no generic, fool-proof way to do this.

Please CadSoft, fix this soon.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 9/11/2013 10:19 AM, James Morrison wrote:

 

It's not that easy Jorge.  If you do that, then internal power planes will

not have cutouts for the milled out area.

  As a result, your pad will be

connected to all the internal layers when you have your board manufactured.

  That means all our internal layers will be shorted together too.  EAGLE

doesn't handle this well and we need much better way to handle these.

Thanks for bringing this up I was aware of it and thought I had put

mention of that in the procedure, I've corrected that now.

 

Right now, the best workaround I have is to add the wires added on layer 46

to layer 20 (dimension) as well.  The copper pouring will honour that and

create openings on internal power planes.  However, this won't work if you

actually do want the pad to connect to those internal pads.  So currently,

there is no generic, fool-proof way to do this.

Don't use the lines on layer 20 since as you've already mentioned it

will mess with the connectivity. The better solution would be to use

cutout polygons on the inner layers so the pours refrain from shorting

to the slot but the autorouter can still reach the pad without incurring

in errors.

 

Please CadSoft, fix this soon.

 

Cheers,

 

James.

 

 

 

Jorge Garcia wrote on Wed, 11 September 2013 14:22

On 9/11/2013 10:19 AM, James Morrison wrote:

 

 

It's not that easy Jorge.  If you do that, then internal power

planes will

not have cutouts for the milled out area.

  As a result, your pad will be

connected to all the internal layers when you have your board

manufactured.

  That means all our internal layers will be shorted together too.

EAGLE

doesn't handle this well and we need much better way to handle

these.

 

Thanks for bringing this up I was aware of it and thought I had put

mention of that in the procedure, I've corrected that now.

 

Right now, the best workaround I have is to add the wires added on

layer 46

to layer 20 (dimension) as well.  The copper pouring will honour

that and

create openings on internal power planes.  However, this won't work

if you

actually do want the pad to connect to those internal pads.  So

currently,

there is no generic, fool-proof way to do this.

 

Don't use the lines on layer 20 since as you've already mentioned it

will mess with the connectivity. The better solution would be to use

cutout polygons on the inner layers so the pours refrain from shorting

 

to the slot but the autorouter can still reach the pad without

incurring

in errors.

 

Please CadSoft, fix this soon.

 

Hi Jorge,

I tried the cutout polygon solution, but that isn't perfect either.  I

would prefer to do that in the library so that I only have to do it once.

But you'd have to put a cutout polygon on every layer.  But on some layers

I could want connectivity so that doesn't work depending on how the device

is connected in the schematic.  Also, I can't recall for sure, but I think

there was a problem if I had a cutout polygon on layer 8 but my PCB didn't

have a layer 8--I think that I got an error in that case and I couldn't add

the device (though I could be wrong about that).

So then you could put a cutout polygon into the PCB, but then you have to

do that for every layer and for every pin EVERY time you insert that part

into a design (if you forget then you'll have fused inner planes).  And if

you have that done perfectly and then move the component you have to

remember to move those other polygons as well--and if you forget you'll get

fused inner layers.  And the worst part is the DRC won't complain about

it.

I think this all highlights why a better solution is required.  It's not

that EAGLE can't make it work.  But when you do this sort of thing there

are way too many places where EAGLE doesn't help and you can end up with a

dead board.  And having a slot for a connector pin (think DC barrel power

plug) is very common-almost on every board I do.  Whatever the solution it

should be able to be specified in the library, work no matter how many

layers there are, and be captured by the DRC when it's not done correctly.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

James Morrison wrote:

Jorge Garcia wrote on Wed, 11 September 2013 14:22

On 9/11/2013 10:19 AM, James Morrison wrote:

 

I think this all highlights why a better solution is required.  It's not

that EAGLE can't make it work.  But when you do this sort of thing there

are way too many places where EAGLE doesn't help and you can end up with a

dead board.  And having a slot for a connector pin (think DC barrel power

plug) is very common-almost on every board I do.  Whatever the solution it

should be able to be specified in the library, work no matter how many

layers there are, and be captured by the DRC when it's not done correctly.

 

Cheers,

 

James.

 

Hi James,

Whenever possible, I've avoided plated ovals and slots in PCBs in the past

because they've always cost an additional arm and leg. I just use an

appropriately sized hole for those crazy rectangular pins, and a little more

solder. That said, I'm an engineer not a PCB designer by trade, and I

haven't been inside a PCB fab facility in years. Are plated slots now common

enough that there isn't much of a difference in cost anymore? I'm curious

what the state of the art is these days. Thanks

Bob

On 9/11/2013 3:03 PM, James Morrison wrote:

 

I think this all highlights why a better solution is required.  It's not

that EAGLE can't make it work.  But when you do this sort of thing there

are way too many places where EAGLE doesn't help and you can end up with a

dead board.  And having a slot for a connector pin (think DC barrel power

plug) is very common-almost on every board I do.  Whatever the solution it

should be able to be specified in the library, work no matter how many

layers there are, and be captured by the DRC when it's not done correctly.

 

Cheers,

 

James.

 

Hi James,

I fully agree, there needs to be a better way because currently all of

the workarounds have pitfalls. The solution will come, I just don't know

how soon.

Let's see what comes out in the next release.

Best Regards,

Jorge Garcia