It's my first time getting a PCB manufactured.

My manufacturer only requires eagle board file, but not a Gerber file. Is it fine to go about getting the board fabricated with them? Or should I be concerned about getting a faulty board made and wasting my money?

  • 4
    \$\begingroup\$ He doesn't sound like a pro company. \$\endgroup\$ – Andy aka Jan 11 '18 at 9:50
  • 10
    \$\begingroup\$ well, there's actually quite a few companies that at least offer to use eagle files (oshpark.com being probably the biggest one, commercially). I don't think that's inherently a problem – but generally, the devices making the PCB do not take eagle files, but Gerbers, and sending a Gerber file that you previewed yourself would give you some confidence that WSIWYG. \$\endgroup\$ – Marcus Müller Jan 11 '18 at 9:53
  • 2
    \$\begingroup\$ He said he doesn't want a gerber and told me to send the .brd file. Probably he can work with other software files as well. \$\endgroup\$ – Harshit Jan 11 '18 at 10:07
  • 14
    \$\begingroup\$ Please clarify: "only requires" means you can still send Gerber, right? so what's the issue? they help novices. Do what you prefer. If they "only accept" Eagle board files, then it's fishy. \$\endgroup\$ – FarO Jan 11 '18 at 12:43
  • 2
    \$\begingroup\$ Is it OSH Park? Because if it's OSH Park, they're great. \$\endgroup\$ – TCassa Jan 12 '18 at 9:00
My manufacturer only requires eagle board file, and not a Gerber file

Run away!

The competency of these people is highly suspect. This is not a real board house. Any minimally competent board house in the world will accept Gerber files.

Some board houses try attracting hobbyists that don't really understand board design and all the Gerber and drill stuff. These board houses will sometimes take Eagle board files as a additional service.

However, even that is not a good idea. Eagle board files don't directly specify all the choices a real engineer makes when exporting Gerber files from Eagle. Take a look at the Eagle CAM processor, and you will see there is choice over what Eagle layers end up on the silkscreen, which board layers to export at all, etc.

You should be the one making the choices and exporting Gerber files from your Eagle design. It's really not hard. It may seem intimidating at first, but it's part of the process you need to learn if you want to design PC boards.

Once you can create Gerber and drill files, you can have your board manufactured at pretty much any board house in the world, including the ones that cater to hobbyists and would have taken your Eagle file. You may even find that such a board house charges less when given Gerber files. In other words, they charge a premium for using the Eagle board file, just don't feature that. If you pass the intelligence test and can supply Gerber files, you get a lower price.

|improve this answer|||||
  • 11
    \$\begingroup\$ What's the problem with accepting ALSO Eagle files? if you don't need advanced control, you save time. If you know what to do, just send Gerber. \$\endgroup\$ – FarO Jan 11 '18 at 12:44
  • 4
    \$\begingroup\$ @Far: As I said, this is not a good idea for you. It's not as simple as giving up some control, when that control ends up making choices for you that you don't want. Without the control, you don't know what will result. As for a board house offering that as a option, I didn't say that was a problem, other than you shouldn't use such a service. \$\endgroup\$ – Olin Lathrop Jan 11 '18 at 19:11
  • \$\begingroup\$ Some of the board houses that most notably offer direct support for Eagle files also graphically render what they will produce so that you can see how they've chewed on your files. I suspect it's been a long time since anyone (especially in the quick turn proto business) fed raw customer-supplied gerbers directly to production machinery, so you're almost certainly going through some preprocessing software even if you send gerbers. Being able to see the result of the preprocessing may be more important than what format you send. \$\endgroup\$ – Chris Stratton Jan 12 '18 at 17:08
  • \$\begingroup\$ @Chris: There are several free Gerber file viewers out there. You can, and should, look over any Gerber files for obvious problems before you send them to a board house. It takes maybe two minutes tops to run the CAM processor in Eagle to make Gerber and drill files from a board. There really is no problem to solve here. \$\endgroup\$ – Olin Lathrop Jan 12 '18 at 17:36
  • 1
    \$\begingroup\$ @OlinLathrop - of course, but that lets you see the gerber files you generated. It doesn't let you see how the manufacturer's software interpreted them and modified them for compatibility with their machinery (let's face it, what's actually in those files is decades old roundabout absurdity with as many flavors as there are generating programs - was just looking at the raw contents of one last week) The board vendors that do show you how they have interpreted your uploads at the time of the order are moving the industry forward. \$\endgroup\$ – Chris Stratton Jan 12 '18 at 17:40

I've been using a very reputable large European PCB house for many years, which accepts Gerber files of course. But they also accept quite a number of PCB design files and do the conversion for no additional charge: I find this very helpful.

My experience with them has been perfect with every Eagle file I've sent, the most complex being 160 x 100 with four layers. There are many things to look out for when making Gerber files; they do this every day, I do it a couple of times a year and it takes me an hour or two to remember everything and check all the details.

For larger runs I use an Asian firm and send them Gerber files because by that stage I want to control the process exactly. Very frequently have to go back and forth a bit about which layer is which and so on.

If for whatever reason you don't trust the firm, find another.

Hope that's helpful.

|improve this answer|||||

There are a lot of possibilities to produce incomplete gerber files from an eagle layout. If your board should have some drill holes too, you need also a NC drill data file in Excellon or Sieb&Meyer format too.

I know board production from the standpoint of designing a board with Eagle and also preparing the necessary files for production from an Eagle .brd file and making a board using the fotoplot and drill files.

If you get layouts from users with very low experience (first or second board), it really makes sense to prefer an Eagle .brd file over Gerber fotoplot files. Errors may be found and corrected much easier (too small traces or pads for instance). There are a lot of PCB samples manufacturers using the .brd file. It is no reason to distrust a manufacturer.

|improve this answer|||||

You could still consider them while sending gerbers if other metrics of their PCB service fit your bill, but sending CAD files to your manufacturer sounds like a bad idea.

From a PCB CAD file in Eagle, Altium, KiCad (or any package of choice), has many references back to the schematic, including a full net list. It's almost trivial to take a PCB CAD design and reverse-engineer it back to a schematic, which is a great aid in cloning your design. This may not be intention of the PCB manufacturer at all; it may be just an extra service; but we may never know.

Note that it is possible to also do this from gerber files, as e.g. Altium can attempt to generate a netlist from a gerber file. However; if you don't write the chip names and resistor values on your board it is highly unlikely one can figure out a design in any appreciable time.

As mentioned by others; exporting production files often has additional design choices. Some designs may draw extra documentation on additional "mechanical" layers that need to be exported on the silkscreen, or intentionally left out. For example some layers can be used as a design aid only, like keep-out zones or outline of modules, or 'pretty drawings' of connectors to indicate their size.

If you're a hobbyist and all you care about is getting your boards manufactured, it may be acceptable. But honestly the "learning curve" of exporting gerbers is nothing extrodinary, and there are many tutorials online telling you how to do it. Additionally, you can check your exported files using free gerber viewers, if you really want to be confident the individual layers are exported correctly.

|improve this answer|||||
  • 3
    \$\begingroup\$ It's not hard to reverse process gerbers to a netlist. The chances of an actual copiers being able to do that are orders of magnitude higher than the chances that anyone will want to copy a beginner's first board. \$\endgroup\$ – Chris Stratton Jan 11 '18 at 18:46

These are the only reasons I can see them wanting that:

  1. If they rejected your gerber file, and wanted the draft so they can make a new one.
  2. If you had proof issues before with them I can see them wanting source files because your program isn't generating it at the correct scale (which i've seen this before).

Now if they wanting it just because, I would look for another board mfg, or at least ask them why they want it. Because, if they are used to catering with the small project community, then they might be on the side of caution, and making sure they have it right. Because a simple setting wrong in your software can throw off the Gerber file.

|improve this answer|||||

Interesting question, with pros and cons on both sides. Bottom line for me: skip the worry with the vendor you have and just go to OSH Park to keep it simple. Here's the summary as I see it:

Pros (reasons to use this board house):

  • save time
  • avoid making errors if you are unfamiliar with generating gerber files
  • fabricators have full access to your design (so they can adjust it as needed for their particular manufacturing process)

Cons (reasons to use a different board house):

  • fabricators have full access to your design (they could introduce errors accidentally, or they could steal your work, though that's unlikely)
  • you don't get to make choices about the way your design gets manufactured
  • you don't get the experience of making gerber files and learning about the process

Overall, I've never heard of a vendor who refused to accept gerber files, so it does sound like a red flag to me. If this is a hobby project, not something you will make a million copies of or something you want to make a lot of money from, then it's probably not a big deal. However, I would highly recommend OSH Park for hobby PCB fab, as they have excellent customer service to help you through the output file generation process. Their prices also can't be beat for low volumes, and they are particularly happy to work with students.

Eventually you will want to find a PCB vendor that you like to work with, maybe someone local to you, and build a relationship with them. Knowing your vendor's particular process will help you a lot with design choices, such as how small you can make your trace widths and spacing, how small you can make your soldermask web, what drill sizes to use, etc. See if you can get a tour of a PCB fab shop so you can understand how the processes work -- it's really fascinating!

Communicating with your vendor is important so you can make sure your design will turn out the way you expect when it's made into a real physical object, not just the idealized image you have on your screen. Vendors really appreciate PCB designers who are willing to work with their requirements, and once you get to know them they will often go the extra mile for you to make sure your boards come out well.

Best of luck with your project!

|improve this answer|||||

I agree with comments posted to your question. There is no reason for a company to ask you for your .brd file if you can export Gerber files.

That being said, it could be that they had bad experience with gerbers from customers and just want to cut out the middle man and make gerber files on their on. It could be that they have some special setup (guessing) and want to import it as they see fit.

Or they just want to steal your IP :-)

Either way, a mail follow-up to this board house would solve your dilemma.

|improve this answer|||||
  • \$\begingroup\$ I actually asked the manufacturer why doesn't he want a Gerber. To this, he replied that his setup can directly take eagle's .brd file. I'm just a bit concerned as this is my first time getting a board manufactured. \$\endgroup\$ – Harshit Jan 11 '18 at 10:03
  • \$\begingroup\$ If it is first time, chances are it isn´t a teleport device so no IP theft hazard. In the end it is your money-your decision \$\endgroup\$ – DeadEye Bojan Jan 11 '18 at 10:05
  • 3
    \$\begingroup\$ If this is your first time getting a board manufactured, the option of letting the board house do the export isn't so bad, actually – especially if they seem friendly, there's a chance that if during export something strikes them as odd (for example, traces too thin, or drills to small or clearances too narrow), they will just tell you! \$\endgroup\$ – Marcus Müller Jan 11 '18 at 10:13
  • \$\begingroup\$ @Harshit That system would be better, because the machine will generate its tool paths with the machine's profile. \$\endgroup\$ – drtechno Jan 11 '18 at 17:42
  • 4
    \$\begingroup\$ If the board house knows this is your first board, they may be trying to minimize their support time for typical newbie mistakes. And you are more likely to get a workable result. The downside though is that you don't learn what you'd need to know to order from a different vendor later. \$\endgroup\$ – Chris Stratton Jan 11 '18 at 18:42

Not the answer you're looking for? Browse other questions tagged or ask your own question.