SparkFun Forums

[thomasew]

Hi,

I recently received a few Eagle files relating to a board I need to make for a university research project. These files are from Germany. I have been trying to get the board manufactured, but I have been running into problems when I send in my gerber files to my manufacturer (4pcb.com). I am getting errors saying Insufficient trace width and missing soldermask clearance. Here are the error descriptions:

Insufficient trace width:
Requirements:We require a minimum of .005" trace width. A premium is charged for spacing or trace width less than .008".

Resolution:All layout packages provide this as a DFM check. Setting sufficient spacing and trace width in your EDA software is the preferred method. Spacing and trace width push and pull against one another, so changing a problem area may require rerouting traces, adding vias, or moving components False errors can be reduced by eliminating title boxes.

The weird thing is that my trace width is 0.032" in Eagle...much bigger than 0.001".

Missing Soldermask Clearance:
Requirements:All surface mount pads should have soldermask relief, or they will be covered by soldermask, and unsolderable.

The customer service desk people sent me this email:

The top layer indicates that the drill symbol drawing has been merged
with the outer layers.
You will need to generate the artwork without any merge toggle turned
on.


I'm not sure what that means. Which toggle is he referring to? All I did when I made the gerber files is open up the cam job from the board file and did an RS-274x job and an EXCELLON job to make 8 gerber files. I made these types of files:

.cmp
.drd
.dri
.gpi
.plc
.sol
.stc
.sts

If anyone has any idea what might be going on and could give me a few pointers, it would be much appreciated. Also, if you need more information, I would be happy to supply that as well.

Thanks

[leon_heller]

Check the Gerbers with GC-Prevue.

Their checking software might have bugs in it. That caused me problems with a board once - there was nothing wrong with it and I found a bug in the Viewmate software the board supplier (Olimex, BTW) was using.

Leon

[thomasew]

view my gerber files with GC-Prevue?

It looks like that only reads .gwk, .xwk, .pwk, and .cwk. Do I convert my gerber files to those somehow in order to check them with GC-Prevue?

[FlipFlops]

The minimum trace width (without additional cost) from Advanced Circuits is 8 mil. Your layout must have some traces that are 5 mil, so you either need to increase the width of these traces, or pay the additional fees.

The missing soldermask clearance probably means that the various layers have become misaligned, or mirrored. When EAGLE runs the cam job you need to make sure that you don't accidentally mirror one of the layers. It could also be a problem with one of the components, and a misplaced soldermask markout, but this is probably not the case. I know the default settings of some older versions of eagle used to have one of the layers set to mirrored by default, and caused a bunch of issues for people.

The list of outputs you have is:

.cmp (top copper)
.drd (nc drill)
.dri (not needed, but excellon drill tool description)
.gpi (not needed, but photoplotter info)
.plc (top silkscreen)
.sol (bottom copper)
.stc (top soldermask)
.sts (bottom soldermask)

I use Advanced Circuits all the time, and never need the .dri or .gpi files. Instead you should have a .drl file (D R L, which is the drill rack file), in addition to the .drd (nc drill) file. Without both the .drd and .drl files you will receive DFM errors.

[leon_heller]

Just rename the Gerber files and drill file to .gbr and .drl files. They have to be imported, you can't read them directly into GC-Prevue.

Leon

[davep238]

view my gerber files with GC-Prevue?

It looks like that only reads .gwk, .xwk, .pwk, and .cwk. Do I convert my gerber files to those somehow in order to check them with GC-Prevue?

As you know, in EAGLE, to produce the board's manufacturing files, you need to run both "excellon.cam" (NC-drill) and "gerb274x.cam" (Gerbers). To view those files in GC-Prevue, click on File/Import and select the files produced by EAGLE's CAM processor. GC-Prevue "knows" that a *.DRD file is an NC-drill file.

FreeDFM.com/4pcb.com will complain that traces are too narrow:
1) if the silkscreen chars are too small. The smallest I use is 0.050" & 16%.
2) if you use copper pours (polygons) the minimum width is 8 mils (0.008").

[thomasew]

I haven't had time today to check these things out, but I'll look tomorrow and report back if something doesn't add up. Thanks for the help.

[thomasew]

Is there a way to look at the sizes of all the silkscreens and adjust the sizes if need be quickly? Or do I have to go to every one and adjust its size independently?

[FlipFlops]

Use the group tool to select all. Next use the smash tool, which will separate the silkscreen from each component.

Use the group tool again to select all, followed by the change tool with the appropriate size you want to change all the silkscreens to.

[thomasew]

Hi,

So I fixed the old problems, but 4pcb now wants an outline layer. I was wondering if someone who is familiar with eagle could explain to me how this is done? The CAM department guy said that they prefer the outline to be on a fab or outline layer or solder mask layer. Also, he said it can't be on a global layer (not sure which layers in Eagle are considered global).

So, does this mean I just draw a rectangle on the solder mask layer? Because I would think that would be interpreted as a solder mask rather than just an outline. Or is there a way to specify a rectangle in a specific layer as being something else? He did say that I should label the outline as such.

Thanks for the help in advance.

[theatrus]

Eagle has an outline layer by default. You should be able to export it as it's own Gerber file (.otl is a common extension)

[thomasew]

Oh it does? I'm not seeing it on the list, but granted there are a lot of numbers not shown on the list. How do I explore the layers that aren't in the drop down list?

[theatrus]

Layer 20, Dimension