Parts misaligned with snap/grid

On 8/28/11 10:26 PM, Steve Klett wrote:

I'm new to Eagle and I'm afriad I may have made a mistake that could cause me some serious trouble.  I have a fairly large (960 parts) schematic.  I've been doing a lot of copying as there are tremendous amounts of repetitive sections of the design.  I'm also using a lot of buses and I don't dry my nets until I have completed naming the buses so that the nets will have a meaningful label.  So I've copied hundreds of parts and at some point I changed the snap/grid settings.  This means I have parts on my schematic that were moved using different grid settings.  The problem now is that when I draw a net it won't snap to the pin of the part I'm trying to use, but rather it will draw the net from the nearest grid point near the pin.  I understand why it's happening but I don't know how to solve the problem.

 

Here is a screenshot of the problem:

  Image:misaligned eagle grid.png

 

>

 

I've tried to find a grid setting that will allow it to work but this requires me to make a grid that is TINY.  To make it worse, when the grid is set really small (<  .0625 in) Eagle ceases to display the net id menu when drawing a net to or from a bus.

 

Have I effectively corrupted my file?  Is there a way to "snap all parts to current grid" or some other repair function?

 

If you select the Move tool and Control-click on the origin of the part

you want to move, that will re-snap it to the current grid. You can also

select a group first and Control-right-click to align the whole group.

Andrew.

I can't seem to make this work.  The part does move a little but the pins of the part still arne't lined up with the grid.  Maybe I need to change the grid to match the specific part's pin spacing?

Am 29.08.2011 04:26, schrieb Steve Klett:

I'm new to Eagle and I'm afriad I may have made a mistake that could cause me some serious trouble.  I have a fairly large (960 parts) schematic.  I've been doing a lot of copying as there are tremendous amounts of repetitive sections of the design.  I'm also using a lot of buses and I don't dry my nets until I have completed naming the buses so that the nets will have a meaningful label.  So I've copied hundreds of parts and at some point I changed the snap/grid settings.  This means I have parts on my schematic that were moved using different grid settings.  The problem now is that when I draw a net it won't snap to the pin of the part I'm trying to use, but rather it will draw the net from the nearest grid point near the pin.  I understand why it's happening but I don't know how to solve the problem.

 

Here is a screenshot of the problem:

  Image:misaligned eagle grid.png

 

>

 

I've tried to find a grid setting that will allow it to work but this requires me to make a grid that is TINY.  To make it worse, when the grid is set really small (<  .0625 in) Eagle ceases to display the net id menu when drawing a net to or from a bus.

 

Have I effectively corrupted my file?  Is there a way to "snap all parts to current grid" or some other repair function?

 

(The png did not make it to the newsgroup)And we are talking about .sch.

There is an ULP "snap-on-grid-sch.ulp" that will move unaligned parts on

grid. Run this ulp with a copy of your *.sch ! You can do perform a snap

on grid also by selecting MOVE, hold down the ctrl-key and then click on

the part or net. This will move the origin on grid and therefore the

pins too. If the pins then are not aligned you have a bad library part.

In .sch the grid is 100mil ALLWAYS and as a beginner you should not

touch this for the next 10 years

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

I too have this problem I am using a maxum library part MAX202ecwe The origin of the part is correctly aligned with the snap grid but the pins are NOT on the grid Does this mean that the design of the part is incorrect

Surly when the part origin is correct, the pins should be correctly aligned also?

The snap to (press move hold control and click on part) has to be done in the symbol editor. Right click on part in schematic go to open symbol and do the snap on, on the pin. Hope this helps!