Confused: Received my first PCB made in Eagle and all resistors are 0603 instead of 0402. What happened?

On 4/01/2015 2:33 a.m., Eric Hold wrote:

So I am new to Eagle PCB.  However, I am not new to electronics as

I've been a repair technician for 25 years.

 

I made my first PCB in Eagle and am disappointed. More to the point: all

of my caps and resistors that were intended to be 0402 ended up with an

0603 footprint size. For example, I used the built-in Eagle library and

selected "R-US_R0402 (R-US_)" for most of my standard resistors--these

ended up being 0603 size. Why?

Also, for the majority of my caps (especially decoupling caps), I also

ended up with 0603 size (where it should have been 0402, just as I

intended).

 

Can anyone explain what I'm overlooking here? I know that the components

I ordered are the correct (as intended size)... like I said, I've been

in this industry a long time, so I know what a 0402 and a 0603 size

component is. Just not clear as to how Eagle defines these.

 

And for reiteration: I did use the built-in Eagle library.

Hi

You will need to do the work determine where the error has been introduced.

Start with your board design.

(1)Use the information tool to verify the package name and library of

the element. This verifies you actually selected the correct part from

the libraries.

(2) If the library and name is correct, establish if the SMD pads sizes

are correct for the 0402 (on the board).

(3)  If they are correct, next check your gerbers using a viewer and

establish if they are correct there. If so the board house did it.

(4) If the SMD pads are wrong on the board but the library name and

package look correct. Then open the library and inspect the device and

the package it uses.

When you post, you should state the version of Eagle you are using as

the libraries differ between versions. In v6.6 I don't see an issue with

the parts you used.

There's also the industry rule that you don't use any library /part that

you have not verified yourself. Once done that part goes into your

personal libraries and you use it from there.

HTH

Warren

Hi Warren,

Been busy, so just responding now...

Using Version 7.2.0 for Mac OS X

(1) I did verify the parts I chose from the library. For example:

Library = resistor

Device = R-US_R0402 (R-US_)

This resulted in all of my 0402 resistors pads being spaced more like a 0603. Strange thing is, I took calipers to measure the pad spacing/dimensions and sure enough, they are a lot closer to a 0603 size. So I don't understand why this part in the library resulted in an incorrect sized pad/layout.

I opened the device and found that the Package attribute = R0402 and the Variant attribute = R0402.

I guess this just leaves me confused and pondering whether Cadsoft Eagle will work for me. I realize that as this is my first time, it would seem that to anyone else, it is likely that I did something wrong--however, I really doubt that this is the case. Someone please convince me to stay with Cadsoft. I'm trying to be rational here.

-Eric

Hi Warren,

Been busy, so just responding now...

Using Version 7.2.0 for Mac OS X

(1) I did verify the parts I chose from the library. For example:

Library = resistor

Device = R-US_R0402 (R-US_)

This resulted in all of my 0402 resistors pads being spaced more like a 0603. Strange thing is, I took calipers to measure the pad spacing/dimensions and sure enough, they are a lot closer to a 0603 size. So I don't understand why this part in the library resulted in an incorrect sized pad/layout.

I opened the device and found that the Package attribute = R0402 and the Variant attribute = R0402.

I guess this just leaves me confused and pondering whether Cadsoft Eagle will work for me. I realize that as this is my first time, it would seem that to anyone else, it is likely that I did something wrong--however, I really doubt that this is the case. Someone please convince me to stay with Cadsoft. I'm trying to be rational here.

-Eric

Hi Eric,

I hope you're doing well. I don't think you did anything wrong in EAGLE.

I think the issue here is that you didn't verify the part for your

purposes. To quote Warren:

"There's also the industry rule that you don't use any library /part

that you have not verified yourself. Once done that part goes into your

personal libraries and you use it from there."

I totally understand that one would expect a package named 0402 to match

closely a 0402 resistor. However not all 0402 footprint recommendations

are the same. The IPC standard specifies 3 footprint variations for each

standard package size (Narrow, Normal, and Wide I probably have the

names wrong).

It would appear that the variant we used is not the one you were

expecting. Different manufacturers will also make variations on this

theme. So there's substantial variability.

With all this said, I do think your board will be able to work. The

bigger pads should allow you to hand assemble the board. That way you

can still use your first PCB.

hth,

Jorge Garcia

"Jorge Garcia"  skrev i nyhetsmeldingen: m98so5$qpi$1@cheetah.cadsoft.de ...

I totally understand that one would expect a package named 0402 to match

closely a 0402 resistor. However not all 0402 footprint recommendations are

the same. The IPC standard specifies 3 footprint variations for each

standard package size (Narrow, Normal, and Wide I probably have the names

wrong).

I could add that it also specifies different footprints based on what

soldering technology to use. Wave soldering requires a lot bigger pads than

reflow. OP simply suffers from inexperience in electronics production. And I

dont think he is alone.

Jorge,

You are absolutely correct, in that I didn't verify my parts. As a new PCB designer, I made the mistake of assuming that the library would be valid. The fact remains: the part clearly called out 0402, while the pads clearly fit 0603 size. I do understand that there are wide variables in types of processes that call for different layout specifications, but this was a case of a poorly written library package/device. Not a big deal though, as I did get the 0402 parts to lay across fine (I also could have put 0603 parts on, but didn't chose to re-order my BOM that way). And the circuit worked gre

My only problem remaining is that even after moving onto my next board, the DRC didn't catch (both first revision and now second revision PCB) an unrouted connection on the PCB. Do you know how this is normally exposed in Eagle? As I start to design larger and/or more complex boards, I want to make sure to minimize mistakes/errors.

Thanks for the help and suggestions! I am happy with Eagle now that I understand library verification.

On 18/01/2015 11:54 a.m., Eric Hold wrote:

 

My only problem remaining is that even after moving onto my next board,

the DRC didn't catch (both first revision and now second revision PCB)

an unrouted connection on the PCB. Do you know how this is normally

exposed in Eagle? As I start to design larger and/or more complex

boards, I want to make sure to minimize mistakes/errors.

Hi Eric

The Design Rule Check does not report air wires as they are not in

breach of design rules.

What you should do is run a ratsnest. It reports the number of airwires

at the lower left in the status line.

Then you have to locate the remaining air wires. If you cannot see them

there are some ULPs that can assist here, like

http://www.cadsoftusa.com/downloads/file/airlist_107.zip

There are many more around.

Check out the other ULPs on the Cadsoft site.

http://www.cadsoftusa.com/downloads/ulps

HTH

Warren