SparkFun Forums 

Where electronics enthusiasts find answers.

Questions about the BatchPCB service

Moderator: robacarp

By pittuck
#4485
thats not at college BTW, when i get home :D :lol:
By pittuck
#4501
okies,

steve can u check the no apertures file.

also oval apertures are now checked.

metric / imperial is not yet in as i have had to restore a webserver this afternoon from a HD with no automated backup/restore files present.

comments should not trouble the drill tool files, drill tool parseing has not been improved. will so soon tho.
By Steve
#4506
Hi Martyn,

So far so good... A gerber file with no apertures at all failed as it was supposed to. It would be nice if a file with one or two missing apertures also failed ;)

What's the issue with oval apertures?

Steve.
By pittuck
#4507
i had not put them in before ;)

just had not got around to it! the widths (overall and wall [for ones with centres cut out]) are checked and the sizes of inside hole are checked.

Missing apertures are on the todo list ;)
By Steve
#4508
You can probably ignore the centre holes in apertures. I've viewed thousands of gerber files and never seen anyone use that feature. The only time I've seen it used was when I created some test data myself to test a gerber rasteriser program.

Steve.[/img]
By Steve
#4509
You can probably ignore the centre holes in apertures. I've viewed thousands of gerber files and never seen anyone use that feature. The only time I've seen it used was when I created some test data myself to test a gerber rasteriser program.

Steve.
By pittuck
#4510
ok well its there.

gotta go now, cause my bain is fuzzled.

btw:

Image

(sorry for using ur bandwidth sparky, as soon as i get my site online i will move the image there!)

U gotta love the number of emails i have accumulated today![/img]
User avatar
By phalanx
#4611
Just tested my board files that I already submitted to Sparkfun and I received an Aperature too thin error message on both of my copper layers. On the other hand, the files passed the Sparkfun DRC and were sent to production.

-Bill
By pittuck
#4612
ok i just looked and the error is on this line:

%ADD10OC8,0.0600*%

This comes down to

%AD - Aperture Desction
D10 - Tool Number
OC8 - No idea! STEVE!
0.0600 - Tool size (this passes)
*% end of line.

the line OC8 is funny

Could u please post a image of the board? (The PCB Viewer program, i.e. a virtual image)
By Steve
#4613
Yes, I know what it is.
%AMOC8*
5,1,8,0,0,1.08239X$1,22.5*
%
%ADD10OC8,0.0600*%
An aperture definition can refer to an aperture macro. See the %AM immediately above the ADD10. An aperture macro is made up of an arbitrary number of 'primitives'.

In this case, the OC8 macro has only one primitive, which is (5) a regular polygon, (1) Laser On (ie: dark, not clear), (8 ) 8 sides, (0,0) centre at 0,0, Diameter $1 which means the first (in this case only) parameter in the aperture definition, and (22.5) rotation of 22.5 degrees.

I don't know why eagle uses an aperture macro to create an octagon when there's a standard octagon aperture... Oh well...

Steve.
User avatar
By phalanx
#4615
Here you go:

Link to Zipped Gerber Files


Top side of board: The crosses showing text origin do not appear in the gerber files.
Image


Bottom side of board:
Image


-Bill
By pittuck
#4637
ok, not 100% sure how i am going to work on them. I will leave it for after release, i will however get it to ignore marco apertures in the next version.

I have uploaded a new version of the drill file and layer checker:

Drill File Checker Updates:

- Metirc / Imperial *Should* now work
- Comments are ignored
- Un-used drills are ignored

Layer File Checker Updates:

- Comments are ignored

hehe,

ok, i will do metric later on the layer file.

There is one known 'bug' in the drill file checker which has exploded into a big one with this release. Here goes:

Drill files like this are OK:

T01C0.012
T02C0.03
T03C0.125

But these are not:

T1F00S00C0.020
T2F00S00C0.035
T3F00S00C0.062
T4F00S00C0.067

Basically at the moment i split from C, so on the top example i get 2 parts in an array of T01 and 0.012, i can then search the rest of the file for T01 (the way the tool T01 is selected for use) and then find out if it is used or not.

BUT with the second example i get T1F00S00 and 0.020, which is fine for size checking, but i need to get the F's and S's removed to check for the tool being used (this file will gove no error as all tools are marked 'unused')

The new line parse function i am working on will give me an array which i can easily search through for the relevant data.

Steve: are the F/S numbers anything to worry about?

Anyhow, thats all for now. I have a paper round to finish, after that i will kick out a bug fix for the above problem. OR work on my nicad smart charger circuit.

Regards,

- Martyn
By Steve
#4642
T1F00S00C0.020
The F and S are feed rate and spindle speed definitions for that tool. They shouldn't be there. No PCB package should put them in a drill file, because they have no way of knowing what the settings should be on the manufacturer's drill machine. They're set to 0 above anyway, so they're useless as well as pointless.

Some CAM software can't handle them and won't import a drill file properly if they're present.

So.. Ignore them :) Or better, strip them out! Actually, I'll have some software ready soon that will assign them to the bit bucket where they belong ;)

Steve.
By pittuck
#4689
okie, bug squashed.

I will do the metric allowances in the layers next.

Steve: the metric / inch codes are same on the drill and layer files right?
By Steve
#4691
Steve: the metric / inch codes are same on the drill and layer files right?
Not necessarily. I mean, they most probably are the same, but I don't think you should rely on that.

There's no guarantee that all the gerber files are formatted the same, either.

I think you should take each file as it comes and not make any assumptions.

*** U ME etc...

Steve.