Have a question about CadSoft EAGLE?  Ask our Expert, Jorge!

On 02/06/2014 02:19 PM, Jorge Garcia wrote:

On 2/5/2014 7:56 PM, Zachary Mink wrote:

     I'm working on a PCB that will involve high dc current as well as

some sensitive digital signals going to a 24-bit ADC.  Would you happen

to have any recommendations or suggestions as resources for a "mixed

signal" board like this?  I've read that analog and digital ground

planes should be separated, but I'm a bit fuzzy on how this is done...

For a 2 layer board it seems like each would be a pour/polygon with some

sort of small trace connecting them?

...

On the board you would draw those polygons in such a way as to overlap

at one point. This will generate a DRC error, that can be safely

ignored. Another option used by many is to create a part that is

essentially to pads shorted by copper, a zero-ohm resistor if you will.

Zachary,

See my post in this newsgroup dated October 1, 2013, titled "Re: Power

and Supply Pin Use on Schematics".  It has a shorts.lbr attached

containing that to which Jorge refers, and an image of using them in a

schematic.  I don't get on the web forums much, but I believe a link to

this would be Power and Supply Pin Use on Schematics

<http://www.element14.com/community/thread/27230/l/power-and-supply-pin-use-on-schematics>.

Using shorts in this fashion assures that the two ground nets are joined

at a single point.  Joining them at two points forms a single-turn

transformer that can resonate at certain frequencies - another source of

noise.  The short can be positioned close to the power supply ground to

minimize the noise crossing from one ground to the other.  You'll still

get a DRC error where the two pads overlap within the short component,

and as Jorge mentioned, can be safely approved.

HTH,

    - Chuck

On 2/5/2014 7:56 PM, Zachary Mink wrote:

     I'm working on a PCB that will involve high dc current as well as

some sensitive digital signals going to a 24-bit ADC.  Would you happen

to have any recommendations or suggestions as resources for a "mixed

signal" board like this?  I've read that analog and digital ground

planes should be separated, but I'm a bit fuzzy on how this is done...

For a 2 layer board it seems like each would be a pour/polygon with some

sort of small trace connecting them?

Hi Zachary,

I'm glad to hear from you. If you must stick to a 2 layer board then the

procedure you have described is exactly what you would do. You would

have two polygons assigned to two different signals (Maybe AGND and

DGND). On your schematic you would assign the various components to the

proper grounds.

On the board you would draw those polygons in such a way as to overlap

at one point. This will generate a DRC error, that can be safely

ignored. Another option used by many is to create a part that is

essentially to pads shorted by copper, a zero-ohm resistor if you will.

For layout suggestions check out:

AN688 By Microchip, it deals with A/D layout

Application Note 139 by Linear Technology, it deals with Power supply

layout.

Let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia

Jorge! 

    I attended your webex to RIT's ARM day and really appreciated the tutorial you presented.  I learned a few tricks that I didn't know before. 

    I'm working on a PCB that will involve high dc current as well as some sensitive digital signals going to a 24-bit ADC.  Would you happen to have any recommendations or suggestions as resources for a "mixed signal" board like this?  I've read that analog and digital ground planes should be separated, but I'm a bit fuzzy on how this is done... For a 2 layer board it seems like each would be a pour/polygon with some sort of small trace connecting them? 

    Thanks for any insight!

On 11/12/2013 03:01 AM, Isaac Tan wrote:

Hi Chuck

 

can you guide me how to use drillcfg.ulp? is it is the setup or is a add

on.

 

Regard

isaac

drillcfg.ulp comes with the distribution.  When you run it, you're asked

for the units for the drill sizes (mm or inch), then you're given the

opportunity to manually add tools, which I never do, then save the file

as a ".drl".

This drill file becomes input to the cam processor (see the -R option)

when building the Excellon drill file.  I usually give the Excellon

drill file an extension of ".exc".

Regardless of the file's extension, you should be able to tell your

board house the layer that is represented by each file, including the

drill file.

HTH,

    - Chuck

Hi,

maybe it is just a more simpler reason... you wrote they can read .drl files. Usually we create Excellon files for drill data and use the file extension .drd. Some people don't recognize this as a drill file and say they want to have .drl instead of .drd. Although the contents of the file is the same, they reject to use it.

Just an idea....

Regards,

Richard

Hi Chuck

can you guide me how to use drillcfg.ulp? is it is the setup or is a add on.

Regard

isaac

On 11/11/2013 06:53 AM, Isaac Tan wrote:

Hi,

 

I got a feedback from them,He had told me that the machine only read the

drill files in the following format:

 

txt

drl

apr

tap

 

The one from Eagle is .drd though.

 

can you help me to check is it possible eagle can generate . txt, drl,

apr or tap file?

Have you tried drillcfg.ulp?

    - Chuck

Hi,

I got a feedback from them,He had told me that the machine only read the drill files in the following format:

.txt

.drl

.apr

.tap

The one from Eagle is .drd though.

can you help me to check is it possible eagle can generate . txt, drl, apr or tap file?

Jorge Garcia wrote:

(...] but I know there are many users that make

PCBs in this manner. Perhaps one of them will chime in.

possibly not with this generic "Have a question about CadSoft EAGLE?

Ask our Expert" subject.

At least in my newsreader they all end up in one gigantic thread.

--

Lorenz

On 11/7/2013 10:31 AM, Isaac Tan wrote:

Hi im helping a university lecturer to ask few question here.

 

she got a PCB Milling Machine from a taiwan company, but she cannot get

the correct gerber file to drill the pcb.is it eagle able to do that?

 

she current using free version, but she claim that she unable to

generate the gerber file from the trial version., is it full version

will unlock this feature?

Hi Isaac,

The free version of EAGLE can generate gerbers, so it's likely that she

is either generating the gerber files incorrectly or that the machine

expects some other format.Chp 9 of the EAGLE manual details making gerbers.

In a nutshell here's the procedure:

1. Open the board layout

2. Click on the CAM processor

3. File -> Open -> Job within the CAM processor window

4. Select the appropriate CAM job (gerb274x.cam is for 2 layers

components on top only, gerb274x-4layer.cam is for 4 layers components

on both sides).

5. Click Process Job

6. For drill file, repeat step 3.

7. Select Excellon.cam

8. Repeat step 5

I would recommend that you look carefully at the type of files the

machine accepts and then go from there. I don't have much experience

with Milling machines myself, but I know there are many users that make

PCBs in this manner. Perhaps one of them will chime in.

Best Regards,

Jorge Garcia