SOT223; Joining pad to tab

Name the poly the same name network connected to that pad has. Via naming button, not via info window.

I've tried this, but it does not work. It does work with other components, but not this type for some reason.

There seems to be only 3 connections allowed on this 4 connection component. I would rather there be 4, even if it means a messy schematic, as this is mainly a board design program. I would rather have to link the tab on the schematic manually to one of the pins to match the component needed.

Can I edit the component to add this?

Which voltage regulator? Tell me how it is called and in what library it is, I'll investigate

Part no. is LD117AS12TR and is a SOT223 in library V-reg.

This one only allows the tab to be connected, but doesn't like the centre leg being attached to the tab. I'm actually using an LM1117 adj one and the datasheet shows this as the tab is the same as the centre leg.

The other problem I had was another SOT223, part no. NDT2995 and is in the zetex library. This is the one I can't attach anything to the tab. Again datasheet shows the tab is the same as the centre leg.

Both give an overlap error if I try.

Thank you for your time investigating it. If there is an alternative part I can replace these with that will allow a neat board using the sot223 then I might be able to do it this way.

I've found someone else had this problem 6 years ago !!! Is this still unresolved ? - How to avoid isolation around a SOT223 collector tab?

You are right, the schematic symbol should have a pin for each pin on the device. You can edit the device to add the pin. You could check the 78L05F device in the Linear library to see how they did it there in the SOT89, but note they connected the 2 pins in the device package.

The LD117AS12TR device in the V-Reg library has an unconnected pad, you can just add a pin to the symbol and connect it in the device window, or create a new symbol with 4 pins.

Thank you for your help. I have finally solved it !

As you say, I've edited the part after finding it in the library and added a pin which was the easy part.  What I had to do then was to "connect" it which was a little complicated and took me a while to find out how.  I saw a "Connect" tab in the lower right window but I've forgotten how I got there. Anyway, this shows you the pins and pad connections. I got confused with the centre panel, as anything in there got added to the top right panel, sometimes with a link symbol, and sometimes a broken link symbol. I'm sure I can find out why eventually, but I did manage to get 4 pins connected to 4 pads, and got a green tick. After saving, this was easy to replace the part I had  - and gave me that extra connection on the schematic. When this was connected, I got an airwire on the board which was correct. Clicking ratsnest filled it in as my ground around the pad with no gaps!

So happy.

One wrinkle is the pin is given a name which I couldn't see a way to edit that at the time, but maybe it is easy to re-name it before I placed it.

On 14/12/2014 2:24 a.m., Richard Perkins. wrote:

I've found someone else had this problem 6 years ago !!! Is this still

unresolved ? - How to avoid isolation around a SOT223 collector tab?

(http://eagle.support.eng.narkive.com/GjWTMXjy/how-to-avoid-isolation-around-a-sot223-collector-tab)

 

--

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

http://www.element14.com/community/message/134705

 

This is not a problem with Eagle these days,

See HELP> Arbitrary Pad Shapes

See the attached. Here I have elected to do away with the SMD for the

tab pad and draw a polygon on the top layer (coloured green so it stands

out). The polygon surrounds the origin of the center pin so is

considered part of it. Thus we have an arbitrary pad shape.

So now you only need three pins for in the schematic symbol that are

connected to the three pins of the package.

When used in the Board editor there are a couple of precautions

dependant on your layout.

The thermals for the centre pin will be extended from the SMD origin so

this will result in only one thermal bridge which will not be enough. In

this case route up from the center pin to the tab and out from there

into the polygon area (three route wires in a 'T' shape) At the top of

the 'T' change the width of the wires to get the desired result.

Alternately turn of thermals for the centre pin in the library  and

manage the thermal connection with the polygon shape of the heat sink area.

HTH

Warren

Attachments:

In the example you gave, there was no electrical connection to the tab. On the examples I gave I couldn't even click or select the pad, as although it had a board pad, putting anything on it created an overlap error. Mine have the pins numbered 1,2,3 & 4 now. If I could do it your way, I would. Tried it, but it didn't work for these two components.

On 14/12/2014 12:51 p.m., Richard Perkins. wrote:

In the example you gave, there was no electrical connection to the tab.

That's correct in so much as you cannot start routing from the centre of

the tab as it is not a SMD pad. The whole pad is the tab and the pad #2.

The only origin for the tab/pad is the origin of the pad so you start

routing from there, and go straight up to the tab. You can stop there if

you like or continue routing out of the tab. At any time you can attach

another route to this initial one by holding CTL and click to start

routing at any point on a routed wire.

Have a look at (pull apart) the attached board. A resistor to ground on

each of the pins. Polygons have ranks.  It does not have DRC errors.

HTH

Warren

On 14/12/2014 12:51 p.m., Richard Perkins. wrote:

In the example you gave, there was no electrical connection to the tab.

That's correct in so much as you cannot start routing from the centre of

the tab as it is not a SMD pad. The whole pad is the tab and the pad #2.

The only origin for the tab/pad is the origin of the pad so you start

routing from there, and go straight up to the tab. You can stop there if

you like or continue routing out of the tab. At any time you can attach

another route to this initial one by holding CTL and click to start

routing at any point on a routed wire.

Have a look at (pull apart) the attached board. A resistor to ground on

each of the pins. Polygons have ranks.  It does not have DRC errors.

HTH

Warren

I have tried other components with this method and it seems simple with those, but I'm sure I was trying the same thing with the two I mentioned, and it just wasn't working. The main difference I see is that the others have the tab numbered 4, so if this is present, then there is no problem. The problem seems to start when the tab is not numbered. Maybe I just found an awkward couple. If you want to check other sot223 devices to find one without that number 4 tab, and try connecting to it.

Well I have learned a lot more by confronting a problem and finding helpful people, and I am still a novice with Eagle, so I expect I will be back with more dumb questions.

Thank you all for your help.

Am 14.12.2014 um 12:39 schrieb Richard Perkins.:

I have tried other components with this method and it seems simple with

those, but I'm sure I was trying the same thing with the two I

mentioned, and it just wasn't working. The main difference I see is that

the others have the tab numbered 4, so if this is present, then there is

no problem. The problem seems to start when the tab is not numbered.

Maybe I just found an awkward couple. If you want to check other sot223

devices to find one without that number 4 tab, and try connecting to it.

 

Well I have learned a lot more by confronting a problem and finding

helpful people, and I am still a novice with Eagle, so I expect I will

be back with more dumb questions.:^0

 

Thank you all for your help.

 

--

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

http://www.element14.com/community/message/134754

 

PADs are what you see in the board and in the packages, PINs are what

you see in the schematic and the symbols. You can connect multiple PADs

to one PIN. This will solve your problem. It has to be done in zthe LBR

editor. If you want to have a heatsink copper area around a PAD without

thermals, just draw a polygon in the board and give it the same name as

the signal the PAD is connected to, and uncheck 'Thermals'. You will see

the checkbox by activating 'INFO' and clicking on the poly.

Ever tried 'help connect', 'help poly' etc?

And, after all, it would be a really good idea to read the manual...