Composite part with "real istic" pads

FeralCl wrote on Fri, 27 January 2017 17:37

I've created a component, a DC-DC convertor.

 

An outline with a few circles and rectangles in layer 21 make a

reasonable looking package, adding four round corner pads results in a

usable part.

 

However the part has four rectangular corner pads, not round pads and

being a bit anal about it I've been attempting to create rectangular pads

but no success so far.

 

Tried overlaying rectangles in the pad layer, overlaying rectangles in

top and bottom layers, creating/overlaying SMD pads top and bottom. Each

attempt has a problem, DRC layer abuse, tracks routed through the pads,

auto-router ignoring the pads even though air-wires show connections.

 

I'm sure there will be a way to doit, but not found it yet.

 

Thanks in advance! Ken.

Hi Ken,

Maybe I am missing what you mean so possibly a picture of what you are

getting and what you want would help. However, if I understand correctly

can you not just go to the properties dialog for each pad (Right Click

Context Menu -> Properties) and then change the roundness setting to say

50%? I just tried that one one of my parts and I got rectangular pads with

rounded corners.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

On 28/01/2017 6:37 a.m., ken wrote:

I've created a component, a DC-DC convertor.

 

An outline with a few circles and rectangles in layer 21 make a reasonable

looking package, adding four round corner pads results in a usable part.

 

However the part has four rectangular corner pads, not round pads and being

a bit anal about it I've been attempting to create rectangular pads but no

success so far.

 

Tried overlaying rectangles in the pad layer, overlaying rectangles in top

and bottom layers, creating/overlaying SMD pads top and bottom. Each

attempt has a problem, DRC layer abuse, tracks routed through the pads,

auto-router ignoring the pads even though air-wires show connections.

 

I'm sure there will be a way to doit, but not found it yet.

 

Thanks in advance! Ken.

Hi Ken

You can change the shape of a pad.

In the package editor display the properties of the pad and change the

'Shape' to square.

Or .. In the package editor click 'Change > Shape > Square and then

click on each of the 4 pads.

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.

rachaelp wrote on Fri, 27 January 2017 17:48

Maybe I am missing what you mean so possibly a picture of what you are

getting and what you want would help. However, if I understand correctly

can you not just go to the properties dialog for each pad (Right Click

Context Menu -> Properties) and then change the roundness setting to sat

50%? I just tried that one one of my parts and I got rectangular pads

with rounded corners.

No, I'm the one missing something.

Easy way is to use non-SMD square pads but they are not rectangular and not

that I want.

Your 50% roundness taken to 0% applied to SMD pads certainly gives correct

appearance but SND pads don't have holes and don't give a PTH in the main

board.

I suppose what i'm asking is how do I create rectangular normal pads with

holes?

Attached is a pic of the component.

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

Attachments:

Sorry Warren, not ignoring you, was composing reply and missed your reply.

I think I covered what you suggest in my reply.

I want rectangular (not square) normal pads that result in a PTH when the

component is used.

Ken

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

Ah right I understand now! I'm not sure that it's possible to create

rectangular PT holes. Would you accept a solution which meant you extended

the pads to rectangles from squares in the layout?

You could have a standard square PTH in the library part and then in the

board draw rectangles top and bottom of the board the shape of the pad on

you want for each PTH. Then name each rectangle with the net name relating

to the pad.

Then draw stop mask rectangles on the tStop and bStop layers to ensure the

mask doesn't cover the area of your extended pads.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

rachaelp wrote on Fri, 27 January 2017 18:50

Ah right I understand now! I'm not sure that it's possible to create

rectangular PT holes. Would you accept a solution which meant you

extended the pads to rectangles from squares in the layout?

Really ? I thought it was just my lack of an imaginative solution (or

limited ability).

Quote:

You could have a standard square PTH in the library part and then in

the board draw rectangles top and bottom of the board the shape of the

pad on you want for each PTH. Then name each rectangle with the net name

relating to the pad.

 

Then draw stop mask rectangles on the tStop and bStop layers to ensure

the mask doesn't cover the area of your extended pads.

What I have currently is small square PTH pads overlaid with rectangles in

the pad layer and t/b/v restricts which seem to be required to stop

unrelated tracks being routed through the pads, maybe because 'Layer Abuse'

DRC errors allow the auto-router to do odd things.

I think your solution is a better way to go but as the sun is about to rise

here I'll try it tomorrow.

Thanks, Ken

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

On 28/01/2017 8:25 a.m., ken wrote:

rachaelp wrote on Fri, 27 January 2017 18:50

Ah right I understand now! I'm not sure that it's possible to create

rectangular PT holes. Would you accept a solution which meant you

extended the pads to rectangles from squares in the layout?

 

Really ? I thought it was just my lack of an imaginative solution (or

limited ability).

 

Quote:

You could have a standard square PTH in the library part and then in

the board draw rectangles top and bottom of the board the shape of the

pad on you want for each PTH. Then name each rectangle with the net name

relating to the pad.

 

Then draw stop mask rectangles on the tStop and bStop layers to ensure

the mask doesn't cover the area of your extended pads.

 

What I have currently is small square PTH pads overlaid with rectangles in

the pad layer and t/b/v restricts which seem to be required to stop

unrelated tracks being routed through the pads, maybe because 'Layer Abuse'

DRC errors allow the auto-router to do odd things.

 

I think your solution is a better way to go but as the sun is about to rise

here I'll try it tomorrow.

 

Thanks, Ken

 

Hi Ken

The 'correct' way to do this would be in the package creating 'Arbitrary

pad shapes'.

In the package editor place your PTH pads, round or square.

Over them on the the layers of interest., top and/or bottom, draw a

polygon that represents the rectangular pad. You will need to take into

account the wire width. You will need to manually address solder mask

and such.

See the manual in your documentation folder. The chapter on Arbitrary

Pad Shapes is what you should read.

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.

warrenbrayshaw wrote on Sat, 28 January 2017 01:31

The 'correct' way to do this would be in the package creating

'Arbitrary pad shapes'.

Yep, do what Warren suggests! For some reason I was thinking that was only

for SMT pads but clearly that wasn't correct and it should work for regular

PTH pads too. So basically if you do as I suggest but in the library itself

(you wont need to name the polygons) then it should be correct for every

time you place the part.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

warrenbrayshaw wrote on Sat, 28 January 2017 01:31

The 'correct' way to do this would be in the package creating

'Arbitrary

pad shapes'.

In the package editor place your PTH pads, round or square.

Over them on the the layers of interest., top and/or bottom, draw a

polygon that represents the rectangular pad. You will need to take into

 

account the wire width. You will need to manually address solder mask

and such.

 

See the manual in your documentation folder. The chapter on Arbitrary

Pad Shapes is what you should read.

Thanks Warren, I'll try try the recommended method.

However it did occur to me that the pad that appears on the package is what

ends up on the board, where a round pad is perfectly acceptable. What I am

trying to achieve is just for cosmetic effect, four pad coloured rectangles

at the package corners.

Ken

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

At last, DRC error free large pads with PTH that auto-route correctly.

Thanks, Ken.

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.