Eagle Drill Sizes

Go to ERC then select the TAB=Sizes, then you'll see "Minimum Drill" set the minimum, but the board needs to be un-routed first.

Depending on what is easier you could also right click on each hole then select the drill size from the menu. That would save you from having to reroute the entire board.

Yes you could, but I find it fundamentally so easy to rip up the board and redo the auto-router, even for the smallest of changes as it only takes a few minutes to re-route.

Depends on the board. Not everything can be auto routed or re-done quickly.

True, true mate, it's just that this is a kid doing a project, so I don't expect it to be to complex!

One could also enter into the command line:

    change drill 15mil

then start clicking on every via.

Even easier yet, enter the following into the command line:

    group all;

    change drill 15mil (C>0 0);

Poof!  all the vias are 15 mils.  The special syntax for typing a mouse

click is explained in the user manual under "Entering Coordinates as

Text" under "Modifier".  This starts on page 97 of the English version

of 7.6.0.

With all that said, it's best to go ahead and use larger vias -

something around a 24 mil for barebones boards.  Advanced circuits can

certainly provide a smaller drill hole, but that doesn't mean that it's

wise to use them.

Things to consider are:

• Physical environment.  Most students, including myself back in the

    day, don't really take adequate precautions to protect a board.

    Metalized mylar bags go a long way to protect against electrostatic

    discharge (ESD).  Plastic chairs and synthetic clothing are the worst.

    Also consider how the board will be transported.  Most likely, it

    will be thrown into a backpack along with a boatload of other books,

    candy bars, breadboards, and other stuff - you know... the usual

    crap that accumulates throughout the course of a curriculum.  It's

    best to keep the board in a metalized mylar bag (ESD protection),

    and insert the bag into a bubble bag.

    Considering the board will most likely be abused (backpacks, etc.),

    one should lean toward using larger vias because as the board flexes

    during mechanical shock and vibration and expands and contracts due

    to temperature changes, cracks can form between the annular ring of

    a via and the through-hole plating leaving a via open.

    Speaking of temperature, note that copper has a significantly higher

    coefficient of expansion than the fiberglass in which it's mounted.

    The via's won't move since they're embedded in the fiberglass, but

    the copper connecting to a via will contract and can pull away from

    the through-hole plating.  The same thing can happen when a very

    narrow trace joins an annular ring associated with a via.  Stress

    can concentrate at the corner where the edge of the trace meets the

    edge of the annular ring.

• Current load is another consideration.  Small vias (about 16mil and

    smaller) are generally suitable for small signals - on the order of

    mA or lower.  Here's a good rule-of-thumb:  a copper trace on 1-oz

    thick copper that is 100 mils wide is equivalent 28 gauge wire.  The

    engineer should consider the current a trace (and via) need to

    carry, its duty cycle, the degree of thermal heating that is

    acceptable, and other environmental considerations.

• I'm not going to go into the transmission line considerations of

    what a change in impedance can do to an RF signal, or the 1/4-turn

    inductor that is formed when a trace goes into a via, and the other

    1/4-turn inductor when it comes out the other side.

I'll bet that some of these considerations come as a surprise.  But you

will get a general feel for what to use where once you've done the

engineering analysis a few times.

For an academic project, I would stick to 24mil or larger holes.  Along

the same lines, stick with the widest trace you can tolerate.  IC's with

0.5mm pin pitch will need 8mil traces, but as soon as you have the room,

widen the trace to at least 10mil.

As you take on a greater variety of projects, you will find that which

size to use when becomes second hand.

This is probably more than what you bargained, and it's certainly more

than what I intended.  But I hope it helps.

Enjoy,

    - Chuck

On 09/30/2016 02:28 AM, Tom Hurst wrote:

Depending on what is easier you could also right click on each hole then select the drill size from the menu. That would save you from having to reroute the entire board.

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/206643

On 30/09/2016 9:11 a.m., Tim Aries wrote:

Hi All,

 

I'm a student currently working on my senior design project. I have no PCB experience whatsoever and this project is my first experience doing a PCB design. I just submitted CAM files to Advanced Circuits to get a prototype board printed for my project (they have special pricing for students) and I got an email back with several errors found by a CAM Engineer. One of the errors include "This design has minimum drill size of .01181" that is less than AC minimum of .015" for $33 special. Please provide a revised drill file"  When I was doing my design I didn't think to adjust any drill sizes so I just used whatever Eagle gave me.

 

In Eagle Freeware, Is there any easy way to change the minimum drill sizes for all the holes under .015"? What is the process of doing this?

 

Thanks in advance!

 

Tim

Hi Tim

Firstly you need to identify where the under size holes are.

Are they in vias or are they in the footprints for the components?

If they are in the vias then you can change them on the board using the

methods the others spoken of. If they are in the footprints for the

components then they need to be changed in the libraries.

So the fastest way to crack this nut would be.

Inspect one via that looks to have a small drill hole and see if it is

undersize. If it is, determine what is a sensible size via drill for the

scale of your design and change all vias to that size.

At this point you will know your vias meet the 0.015 minimum

Next I would run the following ULP

statistic-brd.ulp

When it completes, look on the tab DRILL/HOLE

Look in the columns 'PAD drill' and 'VIA drill'

The values are in millimetres but you will be able to determine if you

have any holes under 0.015" (0.381mm)

Hopefully vias were the issue. If not, come back.

HTH

Warren