Right, when I created gerber files from eagle they all had different extensions, like .sol and .sot and .cpr (these aren't the actual ones, I can't remember off the top of my head)
When I made the gerbers from DesignsparkPCB, it output a bunch of .gbr files.
Do I need to convert them, or is it fine?

 

Hello,

nerdegutta created a blog with a list of PCB houses: PCB board houses
When you look at the sites there are some that exept gerber files.

Bertus

 

Most board houses accept gerber files, and do not care what extension your program stuck on them when they were produced. For example, my Cadence package prefers to name them .art, but they are truly gerber format.

However, for everyone's sanity I always rename them to .gbr.

Do make sure it's RS274X format (no seperate apeture files).

Do include your drill file. Do use Excellion format.

Do include a readme.txt files explaining what may be painfully obvious but explain it anyway. Board size, copper weight, the finish, silk screen ink color, list of files and what each one does, and note any files that need to be inverted.

Here is one random readme file I used to buy boards once:

Artwork 1734A-X2:

This descried the files required for the LED-Top PCB. Layer stackup is in the order of the 
file descriptions.

1734A-X2 and 1734B-X2 are user together in one project. 
See RFQ for additional requirements.

File Name          Description
OUTLINE.GRB        overall board outline .190 by .300 inch. 
                   Some features exceed this outline as noted below 
MASK_TOP.GRB       top side solder mask layer
TOP.GRB            top side copper etch layer
BOTTOM.GRB         bottom side copper etch layer
MASK_BOT.GRB       bottom side solder mask layer
1734A-X2-1-2.drl   plated hole drill file


Notes: 

1 - .02 thick FR4 glass epoxy. 1 oz copper clad both sides.
2 - Finish lead-tin plate & reflow
3 - Silkscreen not required.
4 - Panelization is desired. Manufacturer to determine array based on best use of area. 
    A combination of routing and scoring is desired so pallet can be assembled in one step then
    segmented. 
5 - There are 2 copper etch features on each side that extend to the very edge of the PCB. 
    To make these produceable they have been extended over the edge of thje board such 
    that a later cutting step will leave copper at the edge.
6 - Maximum final board dimensions .190" x .300"

 

Well, yeah...

Huh! The Gerber format is the de-facto industry standard for printed circuit board image transfer. My experience is that they charge extra if you send in files in any other format.
There are two distinct Gerber formats: RS-274X or extended Gerber format and the obsolete RS-274-D. And PCB houses do prefer the RS-274X format
Edit: Here is more about the gerber file format http://en.wikipedia.org/wiki/Gerber_format Gerber files are ASCII based and can be opend in any text file reader. Then delivering files to the PCB house, Check with them if they prefer a naming naming style or not for the files.

 

If a board house doesn't accept gerbers STAY AWAY.

 

Right, when I created gerber files from eagle they all had different extensions, like .sol and .sot and .cpr (these aren't the actual ones, I can't remember off the top of my head)
When I made the gerbers from DesignsparkPCB, it output a bunch of .gbr files.
Do I need to convert them, or is it fine?

@magnet18 - did the Designspark PBC do what you wanted? How would you rate it against Eagle?

 

@ernie, thanks, exactly what I wanted

@magnet18 - did the Designspark PBC do what you wanted? How would you rate it against Eagle?

It did what I wanted, but I would say it's not as easy to use as eagle, and definitely not as advanced.

Also, when moving around the pcb's, there was a ton of lag, which got annoying, but it did the job.