Common BatchPCB Issues

Archive BatchPCB
1

Working at BatchPCB for a month now, I have seen some common problems. Here are some problems and solutions.

Mirrored Bottom Layers:

Look at your files in a separate gerber file viewer (ie: viewplot) to make sure they look right. You can really notice it when you look at the top and bottom soldermask (aka: stop) and drill layers. If there is a drill hole and only one pad of soldermask, you have mirrored layers.

Centered Gerber Files:

This option was made so you could do your own photo etching. The only problem is that it does not do that for your drill data and it become impossible to accurately realign the drill to gerbers. Once again, using a separate gerber file viewer will help you.

Missing Outline:

It is often better to be explicit about the shape of your board than to leave it up to me or some guy working the routing machine at Gold Phoenix. Check your gerber files in a separate viewer and if you don’t see a border, you will get a rectangular board.

DRC Bot:

I understand that a number of people are getting confused by the DRC bot. If you see the warning that says the bot did not recognize your files, don’t worry. Scroll down and you can specify which layer belongs to which file. We are working on upgrading our site and the bot uses some legacy code and we are going to upgrade it too. Currently the DRC bot does not check silkscreen or drill files.

Order Status Says: “Customer Attention Needed:”

We have added this status so that if we encounter a problem with your order, you can see it. If you see this, check your email! We wrote an email to you about your order’s problem.

2

Do you or any of the staff have any thoughts on why the DRC-bot seems to identify many customers’ silkscreen files as soldermask?

My boards come back fine; it’s just the DRC bot that seems to mis-identify the silkscreen gerbers.

I posted a question to this effect once [(link). Now that the Marketplace is open, I see a lot of people seem to be having this problem. Although, I had seen some boards with all layers properly identified, so I wonder if there’s something in my (our) files that the bot is picking up on.

I use pcb version 20070208 on Linux. Looking at my Gerber files, I see every one begins with a comment line like this:

G04 start of page 2 for group 0 idx 0

This was from the back (solder) side copper layer; the numbers are different for each layer; is it possible the bot is reading this comment and using the page number to assign layers? My version of pcb seems to like these page numbers:

Bottom copper: page 2

Bottom silk: page 8

Bottom mask: page 5

Top copper: page 3

Top silk: page 7

Top mask: page 4

Anyone who gets the right layer assignments from the DRC bot: Do your Gerbers have a comment line like this? Different page numbers?

I’m hardly “fluent” in Gerber; are there any other commands I should look for in the files?

Thanks for any help](http://forum.sparkfun.com/viewtopic.php?f=16&t=16610)

3

Take a peek at http://en.wikipedia.org/wiki/G-code#Lis … d_controls

It states G04 is a dwell code, wait for so many ms without axis movement. I’ve seen them used in my gerber files similarly to comments, … I.e.

G04 Layer_Physical_Order=1*
G04 Layer_Color=255*

It appears they’re being used for the editor or CAD application data.

Are you generating RS-247X? or RS-274D?

4

I have done several PCBs on batchpcb before (old site) and had no problems… I tried to submit a PCB design today on the new site - got no email reply from the DRC bot, checking online, it says DRC failed… Looking at the layers, there is no drill view and the filename shows (design name).drl whereas when I uploaded the design, the drill locations were previewed… I tried to re-upload the design under the same name -using edit- after changing the drill file from .TXT to .drl and got nowhere… I also couldn’t delete the design… Is there an instruction file for the new website?? New website is pretty, but not functional, lacks info, and doesn’t seem to be as intuitive as the old one!!

5

I’m seeing the same issues as hormiguero - freshly uploaded PCB design shows DRC failed but no DRB bot email nor details as to why.

6

Same issue here. After being unable to log in, I created a new user account.

I uploaded a new design. The board failed DRC, but no information why.

This board did pass advanced circuits free dfm.

7

same here…i can’t delete my old board designs and my new uploaded designs failed the drc, but i never recieved an email to let me know why. …very frusterating. please post something if anyone finds out how to work around these issues.

8

I’ve tried a few tests and none of my submissions ever come out of “drc: submitted” state. And the displayed board dimensions don’t match the actual files. For one of my tests I added some random text to the back silkscreen layer and the reported board dimensions changed. And the price dropped to match. Nice.

What a mess. Hope this gets sorted out soon.

9

checksix:
I’ve tried a few tests and none of my submissions ever come out of “drc: submitted” state. And the displayed board dimensions don’t match the actual files. For one of my tests I added some random text to the back silkscreen layer and the reported board dimensions changed. And the price dropped to match. Nice.

What a mess. Hope this gets sorted out soon.

I also had the same problem. A loaded the first circuit and all is well. The same circuit with some more text has changed size and fails the test drc. No e-mail help me never arrived. I look forward to updates.

P.S. In general, however, a very good job with batchPcb; D

10

This new DRC bot is simply terrible…I did some testing and I found that it has no issues with overlapping pins from a different net, yet it has issues with the most simple designs that have nothing wrong with them, other than violating rules that are not listed. For instance, the FAQ says 8 mil traces are accepted, but the same design that works with 9 mil traces fails with 8 mil traces. Plus, the email I get is pretty useless. It has no attachment, and just says, “The drcbot has finished processing your BatchPCB upload #93823. Your board has Failed Visit this page to view or order your board”…to order my failed board???

I’m forced to go thru and submit dozens of test designs to figure out just what this new DRC bot will accept, all because the FAQ has no information on what the new DRC bot is looking for.

11

zkummer:
This new DRC bot is simply terrible…I did some testing and I found that it has no issues with overlapping pins from a different net, yet it has issues with the most simple designs that have nothing wrong with them, other than violating rules that are not listed. For instance, the FAQ says 8 mil traces are accepted, but the same design that works with 9 mil traces fails with 8 mil traces. Plus, the email I get is pretty useless. It has no attachment, and just says, “The drcbot has finished processing your BatchPCB upload #93823. Your board has Failed Visit this page to view or order your board”…to order my failed board???

I’m forced to go thru and submit dozens of test designs to figure out just what this new DRC bot will accept, all because the FAQ has no information on what the new DRC bot is looking for.

I agree, this sucks! I’ve ordered several boards about a year ago, now I’m trying to order some more. WTF?

This was such a great service, what happened???

12

Did a bit more testing…

-Pin pads can overlap or touch, even if on different nets…so pads that have 0 or negative clearance will pass, but pads with 1-5 mil fail…and 6mil clearance or higher passes.

-Two pin pads on the same net will pass as long as they are not routed…if they are routed, they fail.

-Accepts as little as 1 mil between copper fill and copper/vias.

-8mil traces are not accepted, but 9+ mil are.

-Traces can have any space between them, even touching or overlapping, even when on different nets.

-Will accept a thermal relief line width of 1 (not sure if this is intentional, but it seems wrong given the minimum trace thickness)

-Board outline of 0 or 9 mil is accepted, outlines of 1-8 mil are not.

-Accepts any annular ring width (even 0) for pins and vias.

…I still have a few more items to check, but once I have done them, I am going to make a blank template for FreePCB and post it here.

13

If anyone who works for Sparkfun/BatchPCB is reading this, please update the FAQ…this is all that is there:

2 Layer sizing:

8mil (~0.2 mm) spacing minimum

8mil (~0.2 mm) traces minimum

20mil (~0.5 mm) minimum drill size

4 Layer sizing:

6mil (~0.15 mm) spacing minimum

6mil (~0.15 mm) traces minimum

13mil (~0.33 mm) minimum drill size

No blind/buried vias

500mil (~12.7 mm) maximum drill size

-4 layer boards not accepted! Middle layers are shown when editing layers, but board shows as 2-layer after that, and seems to be judged by 2-layer standards.

-6mil and less spacing accepted for almost everything on 2-layer boards.

-Will not accept 8mil traces

-Will accept 1mil and 600mil holes.

So, in spite of the fact that the FAQ only lists a few of the basic design criteria needed to design a reliable board, everything in it is wrong! I’ve done testing and found the minimums of everything I work with that will be accepted, but I know for a fact that many of the minimums that the DRC accepts are far too low for production, let alone a reliable circuit.

PLEASE…if anyone with the specs from the manufacturer is reading this, update the FAQ with the following (or at least post it here):

Minimum pad to pad clearance

Minimum pad to trace clearance

Minimum trace to trace clearance

Minimum hole to pad clearance

Minimum hole to trace clearance

Minimum copper to copper fill clearance

Minimum hole-edge to copper fill clearance

Minimum thermal relief line width

Minimum annular ring width for pads

Minimum annular ring width for vias

Minimum & maximum hole sizes

Minimum via hole size

Minimum distance from board edge to any copper

Minimum distance between copper areas

Minimum trace width (if it is 8, please set the DRC to use a float slightly below 8 so they are not rejected)

14

Here is the blank template for new BatchPCB DRC Bot, I made some educated guesses as to what is actually safe for some things, as DRC bot accepts things that are clearly unsafe. This might waste a little bit of board space, but at least the circuits should work. There are some things I cannot put in a template, such as minimum pin size…so a little bit of logic is still required when designing boards. Also, if you want to run a copper area to the edge of the board, the DRC will accept it, but the FreePCB DRC will reject it with this template…in this specific situation, just ignore the errors relating to the copper areas; it will still make gerber files.

15

Much thanks to zkummer and others who contributed. After fighting DRC for a couple of hours I turned to the forums. I noted the exceptions to the DRC checker you outlined, made a couple of very minor fixes and bingo! DRC is now happy. For me all I had to do was change the board outline from 8mil to 9mil since the board was designed with 10/10 rules. I did download your template but cannot import it into my CAD tool set and honestly would rather not download and install FreePCB if I don’t have to. Could I please request you post a written list. Could be text in a reply or txt/csv/??? or other common format. Would be exceptionly helpful and if in a .txt could be edited/added to/etc by others and reposted as a repository that could easily be downloaded but just a written reply would be good too. Thanks again for you efforts to corner this beast as I know all to well how much time you must have put into getting this information. You absolutely saved me lots of hours.

Now the problem is that it thinks my board is 1sq inch when in fact it’s 4.8 sq inches. I’ll continue to read the forums for hints but is seems to me that if they are not going to use lines around the outside (this one is a rectangle) they should put something in the FAQ that tells us how to establish the board outline. I did read everything on the site I could which is why I drew the outline on every layer but no cigar.

Mike

16

PCB rules and limits

Boards can be as small as 0.5" (~12.7 mm) square.

2 or 4 layer boards - 0.062" FR4 material

2 Layer sizing:

8mil (~0.2 mm) spacing minimum

8mil (~0.2 mm) traces minimum

20mil (~0.5 mm) minimum drill size

4 Layer sizing:

6mil (~0.15 mm) spacing minimum

6mil (~0.15 mm) traces minimum

13mil (~0.33 mm) minimum drill size

No blind/buried vias

500mil (~12.7 mm) maximum drill size

All drill hits are plated through

No internal routes, no v-scoring, only drill files are sent to the fab house

Board is routed to the indicated border (very clean edges, you can get creative with the shape as well!)

Soldermask both sides

1oz Copper

No limit on the number of vias

No limit on pads or components

Multiple designs, multiple copies are allowed!

Any size up to 10x15", measured in inch increments (254mm x 381mm)

Minimum billable size 1x1" (smaller boards are allowed but rounded up)

Your design can be any size - 1 inch is the minimum

$10 setup fee (shown as a handling charge) - $2.50 per square inch for 2 layer designs, $8.00/sq. in. for 4 layer designs.

17

Hi,

I’ve been a user of batch since about 2008 and have probably put several scores of boards through about 20 odd orders. However I haven’t used it for about a year since the new website/robot has been running. The reason is that I just don’t have the time to sit down and figure why the bot keeps failing my boards. I always ran DRC on those boards but at the same time I will do RF boards where I want some funny shapes, or I may do something a little weird with copper pours or I may place unconnected vias all over the place so from time to time I’m sure something will get flagged. I had the DRC setup for the old bot based on the website recommendations and was able to get the boards to pass after a bit of experience.

Now today I have a board that I’d like to get done (don’t have enough for a full panel order) and trying batch again a couple of things stand out.

  1. It can’t take metric drill files. I always used metric 3.4 leading and that always worked in the past. Now I did put a board onto the bot and it did actually pass, however it thought it was imperial and quoted me $13,000 for the job.

  2. It gives no feedback. I need some kind of informative feedback from the bot when the bot fails my job. I just put a board through using imperial 2.4 trailing and the layer shots looked just fine and quotes me $15. However it fails, and I have no idea why. My DRC runs through it just fine.

I’d love you use your service again as I put alot of small jobs through it… but as I said I don’t have the time for the run-around. If you could work on your bot to give feedback, I would probably sit down and tweak my DRC.