Eagle PCB Layout Smoothness - Electronic Circuits Projects Diagrams Free

Gayan Soyza · 30th June 2008, 06:06 AM

Hi I need to smooth this PCB layout done from eagle.

The layout is done direct placing the components (not via the schematic) that why it took me 4 hours to draw this

The attachment JPEG file contains the errors I get.

bananasiong · 30th June 2008, 06:43 AM

Hi,
For the track overlapping the pad, it is not the problem. The pad gets the higher priority when it's printed out. As for the pad for the transistor, you can add a bigger pad on it. It is in wirepad library.

Gayan Soyza · 30th June 2008, 06:52 AM

Quote:

Originally Posted by bananasiong

Hi,
For the track overlapping the pad, it is not the problem. The pad gets the higher priority when it's printed out. As for the pad for the transistor, you can add a bigger pad on it. It is in wirepad library.

Hi bananasiong thanks for that I noticed that,when printing directly from the eagle software it prints nicely.

But I need to export the file.When I export the file to BMP it exporting with this overlapping errors thats the problem.

bananasiong · 30th June 2008, 07:01 AM

Hmm.. the overlapping means they are connected. Those not overlapped are not connected actually. If you want them to be not overlapped and connected visually, just remove the wire and reconnect it without touching the hole of the pad.

Gayan Soyza · 30th June 2008, 07:08 AM

Oh no again I have to draw?oooooooooops

There must be a way to solve this.

Quote:

you can add a bigger pad on it. It is in wirepad library.

Nice Library

I searched there is no way to convert the PCB layout directly to the PDF format.

My main point is to export the artwork nicely to some other format

**3v0** · 30th June 2008, 07:18 AM

Quote:

Originally Posted by Gayan Soyza

Oh no again I have to draw?oooooooooops

I searched there is no way to convert the PCB layout directly to the PDF format.

My main point is to export the artwork nicely to some other format

But there is! Use Eagle 5 and proceed as if you were going to print the artwork. In the print dialog box click on PDF, it will create a PDF file of your artwork. A few hours ago I posted a note about using PDF for schematics. Never try to make a PCB using EXPORT>IMGAGE.

If you want larger pads in general increase the size of restring in the DRC.

Also the pads and traces will not generate the overlap error if they have the same name. Check the name of the pad and all traces that connect to it. Change them if needed so they all have the same name.

Quote:

The layout is done direct placing the components (not via the schematic) that why it took me 4 hours to draw this

Nuf said.

Gayan Soyza · 30th June 2008, 07:28 AM

Hi 3v0

Quote:

Originally Posted by 3v0

But there is! Use Eagle 5 and proceed as if you were going to print the artwork. In the print dialog box click on PDF, it will create a PDF file of your artwork.

Oooooooops I'm using Eagle professional edition.Mmmm I like to buy the Eagle 5 (don't know free version allow to do this).Thats really nice If I can export directly to the PDF format.

Quote:

Originally Posted by 3v0

Also the pads and traces will not generate the overlap error if they have the same name. Check the name of the pad and all traces that connect to it. Change them if needed so they all have the same name.

Ah thanks for that I'll try to rename them to the same name.Never tried it yet.

**3v0** · 30th June 2008, 07:34 AM

Quote:

Originally Posted by Gayan Soyza

Oooooooops I'm using Eagle professional edition.Mmmm I like to buy the Eagle 5 (don't know free version allow to do this).

Yes. I use the free version and it works. You could easily do the board you are working on with the free version, the GUI is better to.

geko · 30th June 2008, 09:24 AM

Quote:

Originally Posted by Gayan Soyza

Hi 3v0

Oooooooops I'm using Eagle professional edition.Mmmm I like to buy the Eagle 5 (don't know free version allow to do this).Thats really nice If I can export directly to the PDF format.

Try PrimoPDF writer, it's free to download.

It appears as a printer, when you send a print job to it you get a PDF file. Before Eagle 5.0 I used it all the time.

Primo PDF

Gayan Soyza · 30th June 2008, 09:31 AM

Quote:

Originally Posted by geko

Try PrimoPDF writer, it's free to download.

It appears as a printer, when you send a print job to it you get a PDF file. Before Eagle 5.0 I used it all the time.

Primo PDF

Hi geko thanks for that link.Ya that will be one solution.So that means I can still stuck with Eagle V4

I saw your RGB projects PCB is a PDF version. Was it done with Eagle using PrimoPDF ?That has higher resolution.

geko · 30th June 2008, 09:40 AM

Quote:

Originally Posted by Gayan Soyza

Hi geko thanks for that link.Ya that will be one solution.So that means I can still stuck with Eagle V4

I saw your RGB projects PCB is a PDF version. Was it done with Eagle using PrimoPDF ?That has higher resolution.

Yes, all the PDFs on the site have been done with Primo PDF writer.

As an alternative to Adobe PDF (bloatware) reader try Foxit PDF reader

I believe Foxit also do a free PDF writer but I've not tried it.

Boncuk · 30th June 2008, 09:06 PM

Hi,

I guess you made the routing using a grid size of 1/40". To avoid overlapping errors switch to grid size 1/80" and move the trace connecting the relay to the left by one click. For a 45 deg reference line use either the dimension (20) or the tPlace (21) layer and a trace width of zero.

By moving the trace one click (1/80" (0.3175mm)) the overlap error should be eliminated. For the 45 deg bend use the suggested method or you'll probably trade an overlap error for an angle error.

Pads too small? No problem. Copy and paste the package. Change the pad size and if necessary the drill size and save the package. Create a new device using that package. Erase the old one from the board and use the new one.

If the PCB is created on the base of a schematic it can be replaced without loosing too many of the traces. I have replaced 40pin MCUs without any problem. Just mark the position of the device (package) on the PCB using the above described method, this time marking an X. Place the new and connected device exactly on the position of the old one and use rats nest.

The resulting picture should not leave more than 5mm of trace to route new for each pin, and all air wires going straight into the pin they should connect to.

Boncuk

Gayan Soyza · 1st July 2008, 04:07 AM

Quote:

Originally Posted by 3v0

Also the pads and traces will not generate the overlap error if they have the same name. Check the name of the pad and all traces that connect to it. Change them if needed so they all have the same name.

Hi

I tried renaming the name to same name of the pads & the traces that connect to it.But it always says name already exist.It cannot never renamed

Gayan Soyza · 1st July 2008, 04:19 AM

Quote:

Originally Posted by Boncuk

Hi,

I guess you made the routing using a grid size of 1/40". To avoid overlapping errors switch to grid size 1/80" and move the trace connecting the relay to the left by one click. For a 45 deg reference line use either the dimension (20) or the tPlace (21) layer and a trace width of zero.

Hi I tried to adjust the grid size but it wont allow me to change.

**3v0** · 1st July 2008, 08:22 AM

Quote:

Originally Posted by Gayan Soyza

Hi

I tried renaming the name to same name of the pads & the traces that connect to it.But it always says name already exist.It cannot never renamed

Just open and played with your board. What you are trying to do is a lot like buying an airplane and trying to drive it on the road.

Best
Draw a schematic, when you create the board it will provide air wires for all required traces. Then all you have to do is place the parts and convert the air wires to traces by routing them with the route tool. You then have a board that matches the schematic.

Not So Good
Skip the schematic. Place the parts on the board then connect the pads using the signal tool, this creates air wires. Convert air wires to traces using the route tool. [

BAD (what you are doing)
Skip the schematic. Place the parts on the board. Use the wire tool to draw traces as need. It will make a new signal (name) every time you draw a new trace. Since the pads already have names the traces you connect to them will not be the same name as the pad. That is the source of most of your overlaps.

Air wires are not unique to Eagle. Most good layout packages use them, even without schematic capture. The idea is if you tell the program what you want to connect (draw signal), it will help you place the trace (route it).

I hope this makes sense. If not let me know and I will try again. Once you get the hang of the schematic editor you will not ever want to do a board without first making a schematic.

Thread Tools
Show Printable Version Email this Page
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Title	Starter	Forum	Replies	Latest
Layout instantiation for eagle	bananasiong	General Electronics Chat	3	4th April 2008 04:18 PM
Eagle layout	bananasiong	General Electronics Chat	25	7th October 2007 10:01 PM
Can someone make this PCB layout in Eagle for me?	moody07747	General Electronics Chat	1	27th April 2007 03:45 AM
Eagle layout	zachtheterrible	General Electronics Chat	6	23rd November 2004 08:00 PM
EAGLE PCB LAYOUT users...i nid ur help!	AMPdeck	General Electronics Chat	7	23rd September 2004 06:51 PM

30th June 2008, 06:43 AM	(permalink)
bananasiong	Hi, For the track overlapping the pad, it is not the problem. The pad gets the higher priority when it's printed out. As for the pad for the transistor, you can add a bigger pad on it. It is in wirepad library. __________________ Superman returns..

30th June 2008, 07:01 AM	(permalink)
bananasiong	Hmm.. the overlapping means they are connected. Those not overlapped are not connected actually. If you want them to be not overlapped and connected visually, just remove the wire and reconnect it without touching the hole of the pad. __________________ Superman returns..

30th June 2008, 09:06 PM	(permalink)
Boncuk	Hi, I guess you made the routing using a grid size of 1/40". To avoid overlapping errors switch to grid size 1/80" and move the trace connecting the relay to the left by one click. For a 45 deg reference line use either the dimension (20) or the tPlace (21) layer and a trace width of zero. By moving the trace one click (1/80" (0.3175mm)) the overlap error should be eliminated. For the 45 deg bend use the suggested method or you'll probably trade an overlap error for an angle error. Pads too small? No problem. Copy and paste the package. Change the pad size and if necessary the drill size and save the package. Create a new device using that package. Erase the old one from the board and use the new one. If the PCB is created on the base of a schematic it can be replaced without loosing too many of the traces. I have replaced 40pin MCUs without any problem. Just mark the position of the device (package) on the PCB using the above described method, this time marking an X. Place the new and connected device exactly on the position of the old one and use rats nest. The resulting picture should not leave more than 5mm of trace to route new for each pin, and all air wires going straight into the pin they should connect to. Boncuk Last edited by Boncuk; 30th June 2008 at 09:09 PM.