custom pad shape creation

Ok, I see that there is no way to turn a polygon into a pad. I have added tStop and tRestrict layers and that has solved most of the problems. However, when I export the Gerber files (using RS247X) all of my 'custom pad' shapes appear on the top layer, even though they are clearly set to the bottom layer. .jpg's attached for clarification.

The component package was created on the top layer only. I can't see that this is a problem as the pads that are hidden inside the polygons do appear on the bottom layer, just the poly's that are wrong

hmm, seems I can attach a file so I will have to insert it ...

I have checked the layer selections on the CAM processor and everything looks ok, .cmp = top, pads and vias. .sol = bottom, pads and vias.

Once again, any help appreciated.

On 19.03.2012 11:39, b2lurk wrote:

Ok, I see that there is no way to turn a polygon into a pad. I have added tStop and tRestrict layers and that has solved most of the problems. However, when I export the Gerber files (using RS247X) all of my 'custom pad' shapes appear on the top layer, even though they are clearly set to the bottom layer. .jpg's attached for clarification.

 

The component package was created on the top layer only. I can't see that this is a problem as the pads that are hidden inside the polygons do appear on the bottom layer, just the poly's that are wrong

 

hmm, seems I can attach a file so I will have to insert it ...

 

  Image:eagle.JPG  Image:gerbv.JPG

I have checked the layer selections on the CAM processor and everything looks ok, .cmp = top, pads and vias. .sol = bottom, pads and vias.

 

Once again, any help appreciated.

 

Hello,

again the images didn't make it to the nntp forum.... I looked into the

element14 page and checked the images there. I am not quite sure how you

tried to define arbitrary pad shapes, the images don't have enough

information for evaluation, but may I simply add a test taken from the

EAGLE manual in order to explain how to do this....

The typical way to draw an arbitrary pads shape is:

- Place a PAD or SMD

- Use POLYGON to draw the final pad shape

- For a SMD typically in Layer Top

- For a PAD you have to draw the final shape in all the layers you plan

    to use (Top, Bottom, Inner layers...)

The PAD/SMDs center must be inside the polygon's area. Otherwise

that polygon is not recognized as a part to the pad. Use a reasonable

wire width for the polygon, which fulfils the Design Rules.

- The alternative to POLYGON is WIRE

Start the wire in the origin of the PAD/SMD. You have to draw this

area in any signal layer you plan to use. Please use a reasonable wire

width, which fits to the Design Rules.

- Check the solder stop mask

Mask data will be generated for the PAD/SMD area only. Display

layers 29, tStop and 30, bStop. If you want to have the area not

covered by solder stop lacquer, draw it manually in the appropriate

layer(s).

- Check the cream frame (solder paste mask)

Display layers 31, tCream and 32, bCream for this. As we agreed upon

defining packages always on the top side of a board, the layer we have

to check is 31, tCream. Mask data will be generated automatically for

the SMD area only. If this is not what you would like to have, simply

draw the mask manually. Keep in mind that it is possible to switch off

automatic generation of mask data in the SMD properties (Cream

on/off).

Concerning the layer problem: It mightbe the case that there is a

problmem in EAGLE 6.0.0. You did not mention the version you are

currently using, but I'ld recommend our current beta 6.1.3.

==> http://www.cadsoft.de/betatest/

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

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

Hi!

With the manual addition of cream and stop masks, should I expect an exposed irregular pad in my final PCB after manufacturing?  I want to make the footprint of an inductor (below i include image) so I need this area to be exposed. (I dont know if i just should make a giant rectangular pad, even though the image shows a different footprint).

I have drawn the shape in top, stop mask and cream mask layers. However, when i try to connect the component, the only connection possible is to the smd pad inside the polygon. That is the reason because i fear ending with a rectangular smd exposed inside a big cooper plane.

What should I expect?

Best Regards/ Mit freundlichen Grüssen

Marco Casillas

Hi

I'm facing the same problem.

Please let me know how to create complex shape smd pad, too.

As Marco says,

>I have drawn the shape in top, stop mask and cream mask layers. However, when i try to connect the component, the only connection possible is to the smd pad inside the polygon. That is the reason because i fear ending with a rectangular smd exposed inside a big cooper plane.,

the shape of EAGLE's smd is not changed in response to the shape of polygon.

In moving with move command, I found that the tips of smd pads are not covered in spite of the fact that the appearance of polygon covers except for moving.

How can I resolve this problem?

Best regards

Ishikawa

On 12/7/2015 4:40 PM, Marco Casillas wrote:

Hi!

 

With the manual addition of cream and stop masks, should I expect an

exposed irregular pad in my final PCB after manufacturing?

Yes, the stop masks is what makes the copper exposed.

   I want to

make the footprint of an inductor (below i include image) so I need this

area to be exposed. (I dont know if i just should make a giant

rectangular pad, even though the image shows a different footprint).

 

I have drawn the shape in top, stop mask and cream mask layers. However,

when i try to connect the component, the only connection possible is to

the smd pad inside the polygon. That is the reason because i fear ending

with a rectangular smd exposed inside a big cooper plane.

The SMD pad defines the electrical connectivity so the traces will want

to route to the SMD pad within your irregular shaped pad. Don't worry

though, the manual additions of stop and cream will make sure the whole

pad is exposed.

Let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia

On 12/7/2015 4:40 PM, Marco Casillas wrote:

Hi!

 

With the manual addition of cream and stop masks, should I expect an

exposed irregular pad in my final PCB after manufacturing?

Yes, the stop masks is what makes the copper exposed.

   I want to

make the footprint of an inductor (below i include image) so I need this

area to be exposed. (I dont know if i just should make a giant

rectangular pad, even though the image shows a different footprint).

 

I have drawn the shape in top, stop mask and cream mask layers. However,

when i try to connect the component, the only connection possible is to

the smd pad inside the polygon. That is the reason because i fear ending

with a rectangular smd exposed inside a big cooper plane.

The SMD pad defines the electrical connectivity so the traces will want

to route to the SMD pad within your irregular shaped pad. Don't worry

though, the manual additions of stop and cream will make sure the whole

pad is exposed.

Let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia