Eagle DRC check error: "dimension" and "drill distance"

[earckens]

I get "dimension layer 1" and "dimension layer 16" errors, as well as "drill distance" errors on one component: a 2W10 bridge rectifier. The hole dimensions are 0.031", the pad was auto, now enlarged but still error. The uploads show the DRC settings for "distance": 10mil and 8mil.

I searched myself a heurnia trying to find the cause, nothing found: drill distance, you could not space the holes further apart.. "dimension" error on layer 1 (top) and 16 (bottom)...

This is not the only component I designed myself for the library, but it proves the only one of two with errors (the other is about the same).

 

[ronsimpson]

Please send your library with this part in it.

board: Design Rule Check, size, Minimum Drill = ????

 

[earckens]

Here are the .sch, .brd and .lbr files.

Minimum drill: 20mil
Minimum width: 8mil
Min Micro Via 9.99mm

I used both standard Eagle DRC and Sparkfun DRC, both give same errors.

 

[earckens]

The .brd file is not laid out yet, but even with partial layout I get this error. Or should the board layout be completely finished (sorry, probably stupid question )?

 

[earckens]

Here is a .brd file with fairly laid out board. Same errors.

 

[earckens]

And here the .brd after autorouting: very strange, the bridge rectifier is being ignored..

 

[Pommie]

If you look at the library you will see you have a hole and a pad in each location. Delete the holes and the errors go away. You appear to have the same problem on some capacitors.

Mike.

 

[earckens]

Great! Thank you!
I corrected the error in the package of the bridge rectifier (the capacitors I will take care of), I would never have found this one, kind of like looking very hard for something yet missing the essential.

Now I get "stop mask" errors: what could the reason be there? I did not have this error on the previous .brd?

How can I redo (reset?) the autowire? I had connector X2 rotated 180° but when autorouting now I get error messages...

 

[Pommie]

It looks like you have pads in the stop mask layer. Have you changed the pads on those components?

To ripup all track you can use ripup *.

You might want to add a ground plane to that board. Draw a polygon around your board and add it to the GND net.Then after autorouting click the ratsnest button and you will have a ground plane.

Mike.

 

[earckens]

Hi Mike and others, I found the reason for the "Drill distance layer 20 error" on the 3 capacitors: there was a "dimension layer" conflict with one of the holes. Which was caused by me wantig to have two packages for the same device: a capacitor with holes 0.1" apart, and one package with holes 0.15" apart.
Question: how do I combine these two different packages (each with two pads) in one device (with two connections, but for each package to one different leadlocation)?

To Pommie: no I had not changed the pads on those components. I still need to look into this but this is a very long weekend here, and my missus does not like me sitting around the computer all the time; so it will take a few days before I get to it.

Ripup: ok, works fine.

Ground plane: is the polygon to be drawn with the "wire" tool in the .brd, bottom layer?

 

[JonSea]

To allow for caps of different pitch, there are some footprint in (I believe) the RCL library. You have to connect the 2 common pads together yourself. Here's a pic of the pattern I often use.


I'm short on time this morning, but I'll look up which library this is from later if you can't find it.

 

[JonSea]

This is package C025_050-024X070 from the ref-packages library.

 

[earckens]

Yes I have it, but it took a bit of grey hair to find out I had to use "append" in the "device package connect" part.

 

[earckens]

With the 3-lead package I connected the 2 common pins/pads with the "append" option. Thks JonSea.

 

[earckens]

You might want to add a ground plane to that board. Draw a polygon around your board and add it to the GND net.Then after autorouting click the ratsnest button and you will have a ground plane.

Mike.

In what layer do I draw the polygon? I assume I have to draw this in the .sch? Or in the .brd? I don't quite understand, but would like to do it.

Edit: sorry for the unnecessary post, I found out meanwhile