Problem with Eagle PCB design software.

[Sub MandrelParticipant @submandrel]

Not strictly engineering, but I havea problem with Eagle Light PCB design software that someone may be able to help with?

 

Put simply, eagle refuses to recognise some connections on the board which are OK on the schematic. Other ‘airwires’ it refuses to autoroute, even when these are as simple as two capacitors (large and small) in parallel and the tracks could go where the airwires are. there are no other apparent restrictions.

 

Am I missing something obvious (e.g. have I put things in some sort of ignore layer?) and if so what should I be checking for.

 

Thanks in anticipation.

 

Neil

[Sub MandrelParticipant @submandrel]

[David BlunnParticipant @davidblunn56158]

Posted by Stub Mandrel on 29/12/2010 21:46:34:

Not strictly engineering, but I havea problem with Eagle Light PCB design software that someone may be able to help with?

 

Put simply, eagle refuses to recognise some connections on the board which are OK on the schematic. Other ‘airwires’ it refuses to autoroute, even when these are as simple as two capacitors (large and small) in parallel and the tracks could go where the airwires are. there are no other apparent restrictions.

 

Am I missing something obvious (e.g. have I put things in some sort of ignore layer?) and if so what should I be checking for.

 

Thanks in anticipation.

 

Neil

Hi there, I don’t know much about the application but perhaps your too far from the origin and hence it wont route tracks on the free version.
Also there is a keepout layer that maybe causing the problem, turn on some of the other layers and see if they overlap.

Good luck, Dave

[J A Harvey-SmithParticipant @jaharvey-smith]

Hi,

I’ve not used Eagle PCB software but I’ve many years experience with BoardMaker, EasyPC and various other packages, so I’ll hazard a guess.  This sounds as if the schematic package does not recoginse all the connections you intended to make.  It is likely, for example, that drawing a line on the schematic to meet some other line part way along its length might not be recognised as a join, rather at such a point, three line ends should meet, or there should be a ‘connection dot’ or something similar.

 

Does your schematic software produce a ‘net list’ file? (I bet it does).  These are usually text files readable in notepad or similar, take a look, this will show whether the problem is with the schematic or not.

 

 

 

[Martin WhittleParticipant @martinwhittle67411]

Hi Neil

 

I believe the Eagle light version will not route outside the square defined by the diagonal points (0,0) and (50,50), metric.  You will be able to load larger boards with more layers, created by the ‘standard’ or ‘professional’ versions, but not to work on them much. You can probably draw tracks outside the 50mm square using the WIRE command or button, but not ROUTE.  I suspect it may be possible therefore to generate a larger PCB than 50 x 50mm, but only as a completely manual exercise, without the schematic integration and design rule checking that the program offers.

 

You also cannot ROUTE over an object in the Dimension layer 20, on any tracking layer.  You could WIRE over an object and then connect this track to the relevant net by using the NAME function.  A DRC will then show an error, but this may not matter?  Similarly, you cannot ROUTE over an object in the restriction layers 41 tRestrict and 42 bRestrict, for top or bottom side tracking respectively.

 

On the schematic, I take it that all the wires are correctly drawn on the Nets layer 91, and not drawn on another layer, in which case they would not be electrical connections!  If you MOVE the component on the schematic, you should see all the wiring ‘rubber-band’ and stay connected to the component.

 

There is a helpful message board system on the CadSoft website which you could try.  I have found CadSoft to be responsive to technical queries, but possibly only on the registered (not ‘Light’) versions of the product.

 

Hope this helps

 

Martin

(Occasional user of EAGLE, which I prefer over other PCB design programs I have tried)

[Sub MandrelParticipant @submandrel]

Thanks Folks,

 

It seems David is  right, although I can’t find the ‘keepout’ layer or make it visible, moving things further apart solves most of the issues. It’s strange as it shows the ‘footprint’ of the parts so why two capacitors need a large gap between them I know not?

 

Also I had some surface mount on the top layer and the only easy route to them was on the bottom…

 

JA is right too, although I had already found the error checker which highlights these bits.

 

Martin, the version I have allows 100mm square, just about big enough for my needs (keeps down the cost of pcbs). It tells me and makes a nasty beep if I try to go outside the box. Biggest pain is it won’t rotate a part if that puts a pad outside the box!

 

Your layer 20 issue may be the same as the one David explains.

 

This is steep learning curve software!

 

Thanks for a host of tips!

 

For the record I’m looking at a battery monitor for my Son in law’s van as an upgrade of the one in our camper, and an intelligent nicad charger. Both will use 2x20LCD readouts and be based around an ASVR MEGA8 (strictly the earlier 90S4433 version of it)

 

Neil

[Martin WhittleParticipant @martinwhittle67411]

Hi Neil

 

Components have a physical keepout on layer 39 tKeepout and layer 40 bKeepout for top or bottom side respectively – if these are overlapped it will indicate an error on the design rule check.  This does not affect routing though.

 

Autorouting using the program will not permit track placement which breaks the design rules; manual tracking however can break the design rules (this is not exactly what I said on my earlier message – my apologies!)

 

If you click on the DRC button (or type ‘drc’ followed by ‘enter’ on the keyboard), you will bring up the DRC checker window.  This has a number of tabs along the top, including tabs for various clearances, distances, sizes etc.  These can be edited to suit individual requirements, so if you can accept smaller geometries than the default, you can squeeze tracks into smaller gaps.  The modified settings can be saved as the new default, or as a new design rule .dru file.  One could then have more than one .dru file, e.g. one for tight geometry surface mount boards, and another for larger geometry through-hole boards. 

 

Most PCB CAD software does indeed have a steep learning curve, as you say.  I believe EAGLE to be more friendly than some other programs of comparable capability I have (briefly) tried.  It is worth persevering with.  The ‘help’ files could be more helpful – the manual and tutorial supplied with the registered version are useful.  I do not have the latest version of the program; I am still on v4.16.

 

I occasionally use this for other general-purpose drawing/CAD purposes.  For example I have started to plan a workshop as a pre-retirement project, therefore I have created a library containing cells for some likely sizes of benches and machines, so I can then add such ‘components’ to my ‘PCB’ and move them around to see what fits.  One could equally well make a kitchen planner library, etc.  The components then only have content on the library ‘package’ page, and not the ‘device’ or ‘symbol’  pages; the ‘component’ is then added directly to the ‘board’ and there is no schematic; dimensions are scaled 10:1 as a 16 foot PCB is too large (!); user interface for the board window is switched to a white background.  I think that since the components in this case do not include ‘pads’, the basic allowable size of the ‘board’ <might> then be much greater – possibly the same 64 inch square as for the professional version of the program?

 

Hope your PCB projects go well.

 

Martin

 

[Sub MandrelParticipant @submandrel]

Ingenuity knows no bounds… I use Corel Draw for workshop/kitchen/garden planning! I used to use it for ciruit boards too!

 

I have installed Google Sketchup but find it a bit noddy, perhaps I need more practice?

 

Neil

[Author]

Posts