Eagle does not recognize net lines between user defined part and other components: measurement system incompatibility?

On 21/04/14 20:39, Richard Bonomo wrote:

I had to define a new part on a metric grid (to match the spacings on

its connector).  I THINK I defined the part adequately.

Just to get this absolutely clear (as it's frequently a bone of

contention)...

Because the physical component has metric pin spacing on the package,

you have had to use a metric grid to define the library PACKAGE. You

have ABSOLUTELY NOT had to use metric for the SYMBOL, which has nothing

whatever to do with physical packages and only represents the schematic

notation for the part. This MUST ALWAYS use the 0.1" grid.

 

I have no trouble putting the metric part on my US-standard (inches) -

based project, but when I connect a terminal on the schematic, no

connection (air wire) appears on the board diagram.

All schematic SYMBOLS must be defined on a 0.1" grid to allow the

automatic net connection to the pins. Using a metric grid and putting

the pins on a 2.5mm grid WILL NOT WORK. This is just how it is with

Eagle but it's not a limitation since, as has been remarked many times

and I've just reiterated above, the schematic is a schematic and bears

no relation to physical packages.

 

Could this be due to the mix of units?

 

If you mixed units on the schematic, yes.

On 22/04/2014 7:39 a.m., Richard Bonomo wrote:

I had to define a new part on a metric grid (to match the spacings on

its connector).  I THINK I defined the part adequately.

 

I have no trouble putting the metric part on my US-standard (inches) -

based project, but when I connect a terminal on the schematic, no

connection (air wire) appears on the board diagram.

 

Could this be due to the mix of units?

 

Thank you.

 

Richard B.

When you define a library part you must use a grid of 0.1 inch when

defining the symbol. In that way the pins are on the 0.1 inch grid of

your schematic. The grid you use to build the package with can be anything.

Also ensure you use NET when connecting pins on the schematic.

You will not get an air-wire if you don't successfully connect to the

pin in the schematic. Move the part in the schematic to see if the nets

are attached.

HTH

Warren

Rob Pearce wrote:

On 21/04/14 20:39, Richard Bonomo wrote:

I had to define a new part on a metric grid (to match the spacings on

its connector).  I THINK I defined the part adequately.

 

All schematic SYMBOLS must be defined on a 0.1" grid to allow the

automatic net connection to the pins.[...]

That's not the absolute truth 8-)

The relevant part is: pins must be on grid (in the schematic).

What the grid setting isexactly does not matter.

BUT eagle defaults to a 100mil grid, so using that will save you much

pain.

(Though I use a 50mil grid for symbols with a large number of pins

without problems)

--

Lorenz

On 22/04/2014 6:12 p.m., Lorenz wrote:

Rob Pearce wrote:

On 21/04/14 20:39, Richard Bonomo wrote:

I had to define a new part on a metric grid (to match the spacings on

its connector).  I THINK I defined the part adequately.

 

All schematic SYMBOLS must be defined on a 0.1" grid to allow the

automatic net connection to the pins.[...]

 

That's not the absolute truth 8-)

 

The relevant part is: pins must be on grid (in the schematic).

 

What the grid setting isexactly does not matter.

 

That's not the absolute truth

You could chose a completely obscure size for the symbol grid and then

set to and change all the Cadsoft libraries (any that you wanted to use)

  and all the others around the world  to your custom grid. It will

work.  So it matters what you choose for the grid size if you want to

leverage the work of others.

As Lorenz has done, you can use an even sub-multiple of 0.1" for your

library symbol and then the same sizeed grid for the schematic so the

symbol pins end up on the grid. The 0.1" libraries of the world will

also still work.

All the best

Warren

On 22/04/14 08:13, warrenbrayshaw wrote:

On 22/04/2014 6:12 p.m., Lorenz wrote:

Rob Pearce wrote:

On 21/04/14 20:39, Richard Bonomo wrote:

I had to define a new part on a metric grid (to match the spacings on

its connector).  I THINK I defined the part adequately.

 

All schematic SYMBOLS must be defined on a 0.1" grid to allow the

automatic net connection to the pins.[...]

 

That's not the absolute truth 8-)

 

The relevant part is: pins must be on grid (in the schematic).

 

What the grid setting isexactly does not matter.

 

 

That's not the absolute truth

 

You could chose a completely obscure size for the symbol grid and then

set to and change all the Cadsoft libraries (any that you wanted to use)

and all the others around the world  to your custom grid. It will

work.  So it matters what you choose for the grid size if you want to

leverage the work of others.

 

Yeah, OK, I simplified to avoid confusion. So sue me.

I just checked the definition in the library:  All grids are shown as 0.1" grids.  However, I had defined the package on  a metric grid as the pin spacings do not conform to an inch scale.  Apparently Eagle was smart enough to translate everything to a US inch scale.  When I put an air wire between the metric device and anything else on the board, it put the wire between the "pins" and inserts a 90-degree angle.  In any case, the wire does not get translated to the board drawings.  The automatic internal connections on the package (a consequence of there being multiple power and ground pins) DO show connections on both the board and schematic.   Would anyone care to look at this thing?  Perhaps I am doing something grossly wrong.

OK.   I went back into the symbol and managed to move the pins on the symbol so they actually lined up with the 0.1" grid lines (as opposed to being on an "inch grid" but not actually lining up).  This seems to have done the trick.

Rich