Questions about polygons and merging RECTS in EAGLE

[elektr0]

Hello,

could somebody please help me with the EAGLE PCB tool.

1) Is there a possiblity to merge (boolean add) RECTS, SIGNALS, WIRES within the board tool

2) Eagle does not recognize, that signal parts are connected through other layers by vias ?

Thank you.

elektr0

 

[QELEC]

Re: EAGLE_Problems

Hello.

1.a) You cannot merge RECT with anything in the signal layers (refer to the help about RECT). To merge a rectangular shape with a signal, use the POLYGON tool, and give the shape the same name as the signal.

1.b) You can add signals in the board if no linked schematic is opened. It will make the board and the schematic (if there was one) not consistent.

2) I don't clearly understand your question, but if Eagle doesn't connect directly two wires, or a wire and a polygon, or anything with anything, just begin giving it manually the same name (NAME tool).

I hope it helped.

Regards,

Loïc

 

[elektr0]

Re: EAGLE_Problems

@QELEC

Thank you very much.

So, rectangles (BOTTOM_GND) dont have names, therfore I cant connect pads with rects. But within the GERBER file everything works fine, right ?
All the vias are connected to the backside ground, even if there is still an error within EAGLE, right ?

Does it complicate the GERBER file if I rout many lines within the rectangular shape ?


Thanks

 

[Old Nick]

Re: EAGLE_Problems

use polygons instead of rectangles, and all your problems will be solved.

 

[elektr0]

Re: EAGLE_Problems

Hi,

but polygons are not filled ?

 

[FvM]

EAGLE_Problems

With Eagle, they are either filled or hatched.

 

[QELEC]

EAGLE_Problems

1) Select the polygon tool
2) Choose the options on the top bar
3) Draw it
4) Give it a name (can be done later) if you want it to be connected to an overlapping signal.
5) Click on the "ratsnest" button

If you change the name of the polygon later, click again on ratsnest and eagle will update it directly.

If you want to do a ground plane, just give the polygon the same name as your ground signal (often GND but depends on your design of course). All the ground pads will be connected correctly.

Another comment : if it doesn't look ok in eagle, it will not be ok in the generated gerber files.

 

[elektr0]

Re: EAGLE_Problems

@QELEC

Thank you. I use polygons now.
But I still have problems with the GND plane. It automatically holds a distance to my chip package, because of different nets.

 

[Old Nick]

Re: EAGLE_Problems

I'm not entirely sure what you are meaning, but when you hit 'ratsnest' the polygons will fill and obey design rules (distances from different nets etc.). You can change these in the DRC check dialogue. Also you may want to change the rank on some of your polygons (the higher the number the lower the precidence); this defines which polygon 'moves out of the way' for others (I wouldn't have the highest precidence at rank 2 and further ones at 3,4 etc.)

 

[QELEC]

Re: EAGLE_Problems

About the previous reply from Ol'Nick :

Good precision for the ranks, I hadn't tought about it and I've never used it yet for the polygons.

But I think you cannot change the polygons behaviour in the DRC menu, as the purpose of this tool is only to check the errors. Tell me if I'm wrong. I think it's better to use the polygon options "spacing" and "isolate" (in the top menu bar when you select the poly tool) when you draw it. Or to modify those parameters later with the CHANGE tool.

elektr0, I'm not sure to understand clearly your question. Are you sure the names of the plane and the wires that have to be connected, are the same ? You can attach the .brd file (if it is possible) and I'll have a look if you want.

Have nice Monday,
Loïc

 

[Old Nick]

Re: EAGLE_Problems

About the previous reply from Ol'Nick :

Good precision for the ranks, I hadn't tought about it and I've never used it yet for the polygons.

But I think you cannot change the polygons behaviour in the DRC menu, as the purpose of this tool is only to check the errors. Tell me if I'm wrong. I think it's better to use the polygon options "spacing" and "isolate" (in the top menu bar when you select the poly tool) when you draw it. Or to modify those parameters later with the CHANGE tool.

elektr0, I'm not sure to understand clearly your question. Are you sure the names of the plane and the wires that have to be connected, are the same ? You can attach the .brd file (if it is possible) and I'll have a look if you want.

Have nice Monday,
Loïc

No, you change the rank by clicking on the 'change' icon and selecting 'rank,' and then the level. I'm sorry if that wasn't clear.

 

[elektr0]

Re: EAGLE_Problems

So, thank you all very much.

Now, everything works.
As a conclusion,
1) never use RECTs (also within packages ???)
2) use polygons, the spacing and isolate function helps to define zero spacing to other polygons, etc.

@QELEC: It would be really nice, if I could send you a board file, if I have further questions. It is a really urgent project.

The last real problem with EAGLE we have, is the file import.
Other companies serve dxf (AUTOCAD), ORCAD, ALLEGRO, PCAD, etc.
How can I import such stuff to EAGLE packages or boards ???

Thx. elektr0

 

[elektr0]

Re: EAGLE_Problems

well, i'm sorry but i still got a another question.

How can I improve the accuracy for GERBER 2??? Export.
My polygons are approximated with coarse lines in the GERBER file.

 

[Old Nick]

Re: EAGLE_Problems

I've answered this on your other thread.

You are allowed to click the helped me button, when someone solves your problems you know. There's more chance of them helping you with further questions then.

 

[QELEC]

EAGLE_Problems

About your first question : I've never imported anything to Eagle, so sorry, I cannot help for that.

About the second : the only difference I've noticed between what I see in an eagle board and the generated gerber files (and therefore on the real pcb) are the octogonal pads in eagle, that are ovals in reality. As I don't care about it, I've never searched for the reason. If you're talking about something else, I don't see what it is. My polygons always looked correct until now, exept when I forget to enlarge the dimension lines, in the dimension layers. If a polygon is crossing a dimensional line, it will not be filled correctly. I'm using the job "gerb274x.cam" to generate the gerber files, sometimes modified for the silkscreen layers. And the job "excellon.cam" for the drill files.

I think you can always post a .brd file to be helped here. I'm not always behind my computer and I'm surely not the best experienced eagle user. And also, it can help other poeple to see what we're solving here.