Eagle autorouter

Hi!

Im trying to convert the stepper driver circuit to single sided board.
I have downloaded eagle 5.2.0 for linux. I opened Zach's schematic and board. When I try autorouter ("auto" command) it says, that the light
editor can't perform the requested action.

My questions are:
1. Is it possible to use eagle free edition (aka. light) for autorouting?
2. If autorouting does not supported, why is it the preferred
schematic editor software?

I used KiCAD in the past (it's really hard to learn, and all the symbol contains in one file, thus its almost impossible to share the project with others, or move between linux and windows).

But Eagle isn't easy either.

1) No, not as far as I know
2) because eagle is very common for pcb creation and eagle shematics can be read by each and every creation service

If you don't want the board to be double sided (although you can etch double sided boards pretty well at home) you may try using soldering bridges for crossing paths

'sid

... i made some projects with eagle versions 3 to 4 - it was capable off all actions of the comercial version too. The limitations were: - only 1 sheet per project, 2 copper-layers only and half-euro-format (e.g. 100x80mm).

For bigger boards i used then Target - [server.ibfriedrich.com]

Viktor

> 1) No, not as far as I know

I was not able to autoroute Zach's stepper board v1.1.

However I downloaded a really simple project[1], and I was able to autoroute.

> If you don't want the board to be double sided (although you can etch
> double sided boards pretty well at home) you may try using soldering
> bridges for crossing paths

Yes, this is the way. Just the board need to be modified. (there are many loong traces on the top layer. I need to minimize them.

Hope, I will be done by tomorrow.

[1]: [www.instructables.com]

> ... i made some projects with eagle versions 3 to 4 - it was capable
> off all actions of the comercial version too. The limitations were: -
> only 1 sheet per project, 2 copper-layers only and half-euro-format
> (e.g. 100x80mm).

I tried many pcb software in the past (geda, kicad, protel at uni, and now eagle), none of them was easy to use and intuitive.

I hope Forrest's new pcb software will be different.

Btw, I read somewhere on the blog, that there is somebody who began to write a gcode viewer (or board viewer) in python. Got anyone an url?

Greetings Khiraly et al,

I found a page on a LINUX Gerber file viewer called gerbv: [gerbv.sourceforge.net]
though I haven't yet tried it.
(Note: Gerber format isn't the same thing as Gcode.)

This page lists two other utilities written in python:

>gerber2pdf. A Python script that converts a gerber file 2 pdf.
> Seems quite advanced.

>GerbMerge is also a panelizer, but written in Python.

One of these might be what you were recalling. You might try googling these names, or go to the URL above and search for python and follow the links.

HTH,

Larry

khiraly Wrote:
-------------------------------------------------------
>
> I hope Forrest's new pcb software will be
> different.
>
Mine is super easy to learn, but not nearly as powerful as Eagle (no autorouter). I just got the toolpath routine running.

[vimeo.com]

I'm going to blog this after lunch.

Larry: The python program what Im looking for was written by a reprap member/blogger. (I will search in the archive)

Forrest: Eagle does not have autorouter in the light edition. (maybe it is limited by the number of components too?).
And 80*100mm its really nothing. I modified the stepper controller board to be single sided. And its 80*100mm and some traces are a bit outside of the permitted area


How can I export the board into pdf? I want the bottom side with vias.
I tried the print function but it exports with colors. Although if I cant find the correct solution I will export in color and modify in inkscape after. (I need modify in inkscape anyway, because I want to print 2 board on a single A4 paper).

the colored pdf file:
[khiraly.googlepages.com]

Forrest: Looks good. Cant wait to see your milling in action.
Did you try out your milling bits?

khiraly,
Is it greenarrow's software you are looking for? [objects.reprap.org]

---

[www.hydraraptor.blogspot.com]

khiraly Wrote:
-------------------------------------------------------
>
> Forrest: Eagle does not have autorouter in the
> light edition.
>
Um...

> Is it greenarrow's software you are looking for?

Yes. Thank you.

Ok. I finally figured out how to make proper pdf files.
First, here is my pdf file: [khiraly.googlepages.com]

Short tutorial how to do it:
1. show only the layers what you want to be on the .pdf file. (to check everything is included):
- 16 bottom (the bottom traces)
- 17 pads (the pads of the components)
- 18 Vias (the pads for the soldering bridges)
- 42 bRestrict (four holes in the corners)

2. Select the File->CAM Processor option

2.1 Select in the Output device: PS, scale: 1,
2.2 uncheck the "Fill pads" option
2.3 click on the File button and name your output file: something.ps
2.4 Click on "Process Job" button.

Here is a screenshot:
[khiraly.googlepages.com]

3. convert ps to pdf: ps2pdf14 something.ps
4. open it via inkscape
4.1 clone it: Alt-D, move it to the desired position,
4.2 repeat the above(4.1) step until your page is fully filled with schematics

5. print it on backside of label with laser printer
6. iron it on a pcb
7. etch it

I have done a board, and I propose to add this two layers when printing.

20 - Dimension (the rectangle around the pcb)
52 - bDocu (bottom text (mirrored when printed))

If there is interest, I will make a complete (with photo) tutorial.

Just in case anyone else bumps into this:

Eagle light is just fine with autorouting, but the RepRap boards seem to be designed with a paid edition and probably no one checked if the files work (that is, if it's possible to edit them, not only view and print) with the light edition. Hopefully, the fix is trivial - just select everything ('group' command, drag a box over the whole board) and move ('move' command, Ctrl+right click on the group) to the first quadrant of the work plane (to the top-right of the origin mark that probably was somewhere in the middle of the board or just below it). All in all, Eagle is too dumb to calculate the actual area occupied by the board properly and instead, confines it to the 80x100mm area starting at the origin mark, treating everything that sticks out of it (actually, every origin, pin and pad of an object - the outline of, say, a big connector can be well outside the allowed area as long as no logically significant points are) as a sign that the board is too big.

It would be nice to include a reminder about this somewhere for the people publishing the files to see every time they put things on SF.net, so they can check the board files and fix them if necessary.

>
> but the RepRap boards seem to be designed with a paid edition
>
Either that, or more likely, a cracked edition from over at Pirate Bay. I was sorely tempted to do just that, but refrained and wrote my own.

---

-------------------------------------------------------

Hell, there are no rules here - we're trying to accomplish something.

Opportunity is missed by most people because it is dressed in overalls and looks like work.

Thomas A. Edison

The Eagle free package does have autoroute, but it has some quirks (most CAD packages have their own quirks)

I'm trying to do an all in one CNC PBC design with Eagle at the moment, first time for me.

Absolutely critical:

Don't meddle with the grid size when laying out components... you will put the components out of the connection grid.

These took me ages to find:
edit/net classes: this is the wire widths.
Change, or the spanner icon: No double clicking on eagle like other windows apps, you "change"

How do you know it worked ?
Click the "i" information icon. Then a tiresome box pops up, with all the info, and you actually have to do a second click, so that you can make it go away again.
i.e.-> to thicken a network wire, click the spanner and select class, and the one you want. (only a default one initially)

OK....
Next, when you want to transfer your schematic to a PCB, go File/Switch to board.

You can't do anything to a component, until you have moved (edit/move) it components to within the licienced PCB area.

How do you move the component to the other side of the board ? select layer ? no !
You have to MIRROR it.

A nice feature:
You can move it out of bounds, with the mouse cursor until the cursor goes to the "angle" text box, and manually enter a new angle... i.e. 45deg. YOU MUST THEN press ENTER. After that, right clicking will move it in rotations of 90 deg + your original offset.

Problem:
Any reasonably fine pitched SMD I.Cs, you will have to reset the autorouter grid to a smaller value. Otherwise, the design checker won't let it route the fine detail. If you make the autorouter grid really small, i.e. 2 thousanths of an inch, it will take a long time to complete
I'm STILL trying to get it to route my STM32F103VBT package, the pins are barely bigger than the common commercial smallest recommended trace size.

Graham.

Edit:
I've found that additionally, you have to go Tools/Drc, and then reduce the distances in Clearances, Distances, and Sizes.

Key to it, is that you have to alter the defaults to a higher density setup in both the autoroute Grid, and the DRC settings, so that Eagle can "give itself permission" to route with reduced clearances.

If you look at the attached, you can see that with many of the clearances reduced, and the auto route grid down to 4mil, the default autorouter settings allow it to complete around the low density pad area, and to complete about 50% of the routing from the high density area (the TQFP 100 pin package.)

I suspect, that I need to tweak the via permissions somehow, to allow a higher completion. Being a microcontroller, of course I also have some flexibility over which pins I use for which purpose, so I could swap things around on the schematic also. I have a lot yet to complete though, general purpose I/O, protected analogue inputs, oscilator, Power in, regulation down to 3.6V for the STM32 micro, decoupling, JTAG programming port, USB and/or RS232, RS485... possibly. Also, you may note the traces around the L298 dual full bridge drivers are pathetically small, These are auto routed from a net that is inferred at the schematic stage, so I have to find where the tweak is, and correct them. I need some resistors in series with the steppers too, a matter for some research...

I'm working within the limitations of the free version, so the PCB is limited in size. In this case, I would power the steppers off 5 volts initially, as it's less smelly on the electronics if something goes wrong

Any tips welcome, I'm new to eagle, and I'm stronger on the SW side than the HW, although I did run my own design/programme/build business for 4 years, a while back.

By the way, the dual SIL packages just above the L298 s are SIL full wave bridge rectifiers, I'm hoping to use them for protection of the L298 s from recirculating current from the stepper motor coils, although I'm not 100% sure that their response time is up to it... Tidy solution otherwise.

Graham.

Edited 1 time(s). Last edit at 01/21/2009 02:17AM by grael.

i can't make the width of autoroute larger. change width no affect

khiraly Wrote:
-------------------------------------------------------
> ...
> Forrest: Eagle does not have autorouter in the
> light edition. (maybe it is limited by the number
> of components too?).
> And 80*100mm its really nothing. I modified the
> stepper controller board to be single sided. And
> its 80*100mm and some traces are a bit outside of
> the permitted area
> ...
You could compile the Eagle OSS version which you can download from Cadsoft [www.cadsoft.de]
The 5.4.0 version does Autoroute the stepperboard, at least on Mac OS X that is.

Regards,
Johan