Multiple(non standart) footprints

On 25.05.2012 21:10, Nifril wrote:

Good Day. I have a two questions: 1) I want to put several different

footprints on the PCB for one part on the scheme.  For example

ATmega32U4 in QFN/TQFP package or a trimmer in vertical/horizontal

package. How can I do this?

Hi,

when you create a Device in the library you can assign different

package variants. Therefore you have to click onto the "New" button

and choose a package from the list. Be sure to type in a variant

name, as well. Then click OK and the package available. When you

click onto "New" again, you can select another package.

 

2) In my scheme I have a  transistor which I need put on the big heat

sink. Transistor will be connected  to the connector on PCB. How can

I add a part on the scheme but hide them on the PCB?

 

You could define a kind of dummy part that has no real pins in the

symbol. So you do not have to assign a package. You could place vias

in the layout then for connecting the transistor with the board.

Alternatively use a transistor symbol and assign it to a connector

package.

Hope this helps.

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

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

On 05/25/2012 03:10 PM, Nifril wrote:

Good Day.

I have a two questions:

1) I want to put several different footprints on the PCB for one part on the scheme.  For example ATmega32U4 in QFN/TQFP package or a trimmer in vertical/horizontal package.

How can I do this?

I have done the same thing on several occasions.  Once you have your

part established with the desired footprints in the library, you need to

add the part to the schematic twice - once for each footprint.  You can

place both symbols directly on top of each other do that all connections

will be identical.  I smash the symbol and move each reference (U1, U2,

or R1, R2) so they don't overlap.  I then add a note to the schematic

that only one of the two parts will be populated.

 

2) In my scheme I have a  transistor which I need put on the big heat sink. Transistor will be connected  to the connector on PCB.

How can I add a part on the scheme but hide them on the PCB?

There are a couple of ways to approach this determined by whether or not

you want to show the connector in the schematic for BOM purposes or not.

If you want to show the connector, the add the connector as expected in

your schematic.  In your library create a device that has just the

symbol of the transistor - no packages defined.  Then add that device to

your schematic.

In the case where you do not want to show the connector, you can create

a variant of the transistor device that has the connector's footprint,

then add that device/package to your schematic.

HTH,

    - Chuck