Arbitrarily shaped SMD polygons not accepting traces

On 11/06/2017 4:43 a.m., Ansen Seale wrote:

I've made some polygons around SMD pads to create some thermal relief for my parts. The problem is that I can't manually route and traces into these polygons. The trace avoids the perimiter of the polygon and won't let it in to be connected.

 

There doesn't seem to be any Restrict or Keepout information, so I don't know what I'm doing wrong.

 

Thanks for any suggestion!

 

--

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

https://www.element14.com/community/message/223807

 

HI

Normally you would create arbitrary pad shapes around SMD and pads in

the package editor. You oan place polygons around SMD and pad on the

board but you will need to name the signal polygon the same as the

signal attached to that pad/SMD. Also you need to manually the create

the solder mask and solder cream in the area of the polygon as it will

not be created automatically.

HTH

Warren

--

... use NNTP://news.cadsoft.de and a functional news reader like

Thunderbird!

... or http://www.eaglecentral.ca browser access to CadSoft EAGLE

support forums.

---

This email has been checked for viruses by Avast antivirus software.

https://www.avast.com/antivirus

Hi Warren,

Yes, I'm creating this in the package editor of the library. The polygon completely surround a valid SMD. The polygon does not seem to have a name in the Properties info box and I cannot use the name tool to click it to change it's name.

Ansen Seale wrote:

 

Hi Warren,

 

Yes, I'm creating this in the package editor of the library. The polygon completely surround a valid SMD. The polygon does not seem to have a name in the Properties info box and I cannot use the name tool to click it to change it's name.

Hi Ansen,

What version of EAGLE are you using?

Best Regards,

Rachael

On 06/11/2017 11:02 AM, Ansen Seale wrote:

Hi Warren,

 

Yes, I'm creating this in the package editor of the library. The polygon completely surround a valid SMD. The polygon does not seem to have a name in the Properties info box and I cannot use the name tool to click it to change it's name.

 

Ansen,

I have run across this as well in v7.7.  It seems that despite the pad

being an arbitrary shape, the only hot-spot to which or from which one

can route is the center of the SMD.

This behavior is different than a polygon defined in the board editor.

In that case, one can route to anywhere inside the polygon and it is

considered a connection.  i.e. The air wire is no longer present.

I do not know of a way to terminate a wire inside a library-defined

polygon and still have it considered a connection.

HTH,

     - Chuck

On 12.06.2017 14:19, Chuck Huber wrote:

On 06/11/2017 11:02 AM, Ansen Seale wrote:

Hi Warren,

 

Yes, I'm creating this in the package editor of the library. The polygon completely surround a valid SMD. The polygon does not seem to have a name in the Properties info box and I cannot use the name tool to click it to change it's name.

 

 

Ansen,

 

I have run across this as well in v7.7.  It seems that despite the pad

being an arbitrary shape, the only hot-spot to which or from which one

can route is the center of the SMD.

 

This behavior is different than a polygon defined in the board editor. 

In that case, one can route to anywhere inside the polygon and it is

considered a connection.  i.e. The air wire is no longer present.

 

I do not know of a way to terminate a wire inside a library-defined

polygon and still have it considered a connection.

 

HTH,

      - Chuck

Hi Ansen,

you can add an additional hot-spot to a SMD or pad by adding a wire

already in the package.. The wire has to start or end at the SMD's

origin.

s.a. Help PAD/SMD section "Arbitrary Pad Shapes"

especially "A wire in a signal layer is considered connected ..."

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl -- EAGLE Support

On 12.06.2017 14:19, Chuck Huber wrote:

On 06/11/2017 11:02 AM, Ansen Seale wrote:

Hi Warren,

 

Yes, I'm creating this in the package editor of the library. The polygon completely surround a valid SMD. The polygon does not seem to have a name in the Properties info box and I cannot use the name tool to click it to change it's name.

 

 

Ansen,

 

I have run across this as well in v7.7.  It seems that despite the pad

being an arbitrary shape, the only hot-spot to which or from which one

can route is the center of the SMD.

 

This behavior is different than a polygon defined in the board editor. 

In that case, one can route to anywhere inside the polygon and it is

considered a connection.  i.e. The air wire is no longer present.

 

I do not know of a way to terminate a wire inside a library-defined

polygon and still have it considered a connection.

 

HTH,

      - Chuck

Hi Ansen,

you can add an additional hot-spot to a SMD or pad by adding a wire

already in the package.. The wire has to start or end at the SMD's

origin.

s.a. Help PAD/SMD section "Arbitrary Pad Shapes"

especially "A wire in a signal layer is considered connected ..."

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl -- EAGLE Support

Thanks everyone. I have found a workaround for this bad behavior. You can start your route from the SMD in question and exit the polygon, but you can't go the other way. The router will complain with the "no go" icon, but it will lay down a trace anyway.

On 12.06.2017 15:12, Richard Hammerl wrote:

On 12.06.2017 14:19, Chuck Huber wrote:

I have run across this as well in v7.7.  It seems that despite the pad

being an arbitrary shape, the only hot-spot to which or from which one

can route is the center of the SMD.

While at it, there is an annoying optimize side effect of this. If you

draw two same width, same layer wires in the opposite direction from

this smd, they may all of a sudden get optimized, and no longer end up

in the smd. The optimize seems to happen after any move of the wires

ends, and possibly after other actions too. This bug has annoyed me a

lot, and I guess it is some optimize leftover shared with the board editor.