Author Topic: PCB Rejected (Read 29363 times)

snipersquad100 · « **on:** May 23, 2014, 02:24:23 pm »

Hi, I am a hobbyist in electronics, I've made my own doggy pcb at home in the past that worked quite well but recently I decided to go one step further and get one made from a pcb house. I made "another" constant current dummy load and used eagle to design the board. I saw in one of Daves mailbag video's I think it was mentioning easyEDA, so I thought id give them a go. I sent the eagle gerber files off to them today but they refused to make it. They said "Hi, After I reviewed your board, I can't make it done, this board will lost your money and time. If this is your first time try to build a PCB. You should try to make it better."
I will post a pic of the board here, if someone can tell me what I'm doing wrong I be grateful.

I know I'm not a pro in designing pcbs, to me its just a bit of fun. If im willing to pay to get it made I cant see why they wont do it.

snipersquad100 · « **Reply #1 on:** May 23, 2014, 02:55:43 pm »

Defo easyEDA, they do their own pcb software as well as manufacture pcb'shttp://easyeda.com/cms_files_easyeda-pcb-fabrication-prices-capabilities.htm and also allow you to import other software like eagle, Ltspice ect, They even said I could just email them the eagle gerber files. the design check was ok no errors, drill size were just 3,4 and 10mm

ConKbot · « **Reply #2 on:** May 23, 2014, 02:57:49 pm »

Only cost increasing things I see are:

Non plated though holes. Drilled holes that arent plated requires a separate drilling step. Though the bigger hole could be routed if they support internal routing.
Thin traces. How wide are the little traces going to/from the SMD resistors? Unless you have a reason to, I'd say dont go below 12/12 traces/spacing so even the least capable board houses can do it. Some places charge more for finer traces, so 8/8 may be one price tier, but 6/6 may be another
Vias: I cant really see the center hole size of the vias. How big is it? Dont go below the minimum drill size, otherwise they have to be laser drilled microvias. Another step, adds cost.

Though I still feel a little slow this morning :p
Also, get rid of your floating islands, or put vias down to connect them to ground. Not a DFM issue, and probably wouldnt be an issue in that circuit, but definitely not good practice.

c4757p · « **Reply #3 on:** May 23, 2014, 02:58:53 pm »

Did you actually check the Gerbers? There are a lot of options when generating them. You should always open and inspect them in a separate Gerber viewer.

snipersquad100 · « **Reply #4 on:** May 23, 2014, 03:12:10 pm »

Thinest trace is 16mil, the centre hole is 10mm just to fasten a 10 turn pot to the pcb. I didn't check the Gerbers I don't know how.

c4757p · « **Reply #5 on:** May 23, 2014, 03:16:01 pm »

Quote from: snipersquad100 on May 23, 2014, 03:12:10 pm

I didn't check the Gerbers I don't know how.

You can just load them into any old Gerber viewer.

There are a few online. This one works nicely. This one should give a nice, 3D render, but seems to just fart and make rude gestures at me when I load my (KiCad) Gerbers into it. There's also this one.

Then there's gerbv, part of gEDA, and KiCad has GerbView. Eagle probably has a viewer as well. ZofzPCB is an awesome 3D viewer that lets you actually navigate through the stackup.

Try to open them in a few different viewers. Gerber is an odd format... And load up the drill file too.

snipersquad100 · « **Reply #6 on:** May 23, 2014, 03:18:41 pm »

Thank you c4757p, I will have a look.
cheers

mamalala · « **Reply #7 on:** May 23, 2014, 03:31:49 pm »

It would be more helpful if you could attache a ZIP file with the Eagle .brd in it. The image is rather small and makes it hard to figure things out. Plus, it doesn't tell squat about what layer have been used for what, etc.

Greetings,

Chris

snipersquad100 · « **Reply #8 on:** May 23, 2014, 03:39:22 pm »

Cant upload that type of file to this forum.

snipersquad100 · « **Reply #9 on:** May 23, 2014, 03:43:18 pm »

let me try this.

Dago · « **Reply #10 on:** May 23, 2014, 03:53:45 pm »

Gerbv is also a decent viewer. http://gerbv.sourceforge.net/

zapta · « **Reply #11 on:** May 23, 2014, 03:55:35 pm »

You can upload your eagle.brd file to http://oshpark.com/ , it will process it for 10-30 seconds and then you click Continue and it will let you view the various layers it extracted. It's free.

If the design indeed has problems it is nice of them to let you know in advance (though they could be more specific).

kc0ngu · « **Reply #12 on:** May 23, 2014, 03:57:49 pm »

Hi,
Your .brd file looks OK in Eagle, but, as others have said, really need to look at the Gerber files to see what may have caused the rejection. Your gerbers will show if the silkscreen is in the copper layer or something like that has happened, it's easily done. Did you use a Gerber CAM file supplied by the pcb manufacturer or someone like Sparkfun or did you just run your own Gerber CAM?
The comment from the board house sounds like they did not like your design, which is your business, not there's.
Hope you can get it made somewhere,
Regards

nctnico · « **Reply #13 on:** May 23, 2014, 04:09:07 pm »

A good PCB manufacturer will send you a picture and/or document showing/explaining the problem in detail. I have good experiences with Eurocircuits and SeeedStudio.

mamalala · « **Reply #14 on:** May 23, 2014, 04:14:10 pm »

Quote from: snipersquad100 on May 23, 2014, 03:43:18 pm

let me try this.

OK, that worked.

A few notes: Make the traces wider. Also, you can reduce the isolation between traces and copper fills. As has been mentioned already, stitch the top & bottom GND planes together with via's. To do so, place a single via, give it the name "GND", then click on "ratsnest" to make sure it really connected them and that you didn't make a mistake. Then copy that via and place the copy, repeat until you have enough of them

On the part labelled D1 you have a dead trace on pin 3, which is connected to nothing. You can move around a lot of the parts easily so that you don't have to do all those jagged traced. You can also change the via shape to round. Check what the restring requirements of the PCB fab are, many also provide a DRC that should set the proper values.

Get rid of the _tsilk and _bsilk layers that you added in yellow. That's what the tPlace and bPlace layers are for. Everything in a part outline that crosses a solderpad should go to the respective tDocu and bDocu layer instead. Your big center hole for the potentiometer is problematic: First, you usually have a index-notch as well, or a D-shaped hole as an alternative (depends on the type), as to avoid having the whole pot spin around (yes, screws/nuts can come loose, after all). Then you have parts and traces way too close to that hole. How dou plan to mount the pot of these things are in the way, i.e. no suitable clearance is available? Same goes for some of the other holes. Screw-heads are larger than the screw....

Attached is .cam file that you can load to create the Gerber file set plus the Excellon drill file, for 2-layer boards.

Greetings,

Chris

snipersquad100 · « **Reply #15 on:** May 23, 2014, 05:24:40 pm »

Thank you for your comments, I will redo the board and let you know what happens.

tszaboo · « **Reply #16 on:** May 23, 2014, 05:49:57 pm »

I think first you should try sending it to a different manufacturer where they speak english.
Eurocircuits has an online gerber viewer, which has a built in DRC checker. Upload your zip to them, it will tell you what is the problem.

snipersquad100 · « **Reply #17 on:** May 23, 2014, 06:23:01 pm »

thanks nandblog

Kjelt · « **Reply #18 on:** May 23, 2014, 09:46:53 pm »

Also if it is a load and the fets will be used in linear operation do you want to cool them? Just a thought.

snipersquad100 · « **Reply #19 on:** May 23, 2014, 10:01:38 pm »

Hence the fets are lind up with mounting holes for the heatsink.

Rory · « **Reply #20 on:** May 24, 2014, 01:13:57 am »

Consider thermally isolating your component ground side pads from the ground plane that's flooded around them. Same for the through-hole pads. It makes rework/repair/replace so much easier.

snipersquad100 · « **Reply #21 on:** May 24, 2014, 10:27:58 am »

Just found someone to manufacture my board www.smart-prototyping.com, 10 boards for $21 inc postage bargain, just hope price don't influence the quality, but hey its go to be better than home build pcb's. I will let you know when they arrive.

tom66 · « **Reply #22 on:** May 24, 2014, 10:33:06 am »

In general I've found boards from seeed-studio, itead, etc. to be of OK quality. I wouldn't use them down to 6/6 but I'd trust them with 8/8 and a few more mils on the drill holes. Their biggest weakness is the drill hole alignment, it's often off by a few mils which can make a difference if you're using small vias. Also don't bother too much with the silkscreen below 8/8 because it's just not high enough resolution to work.

tszaboo · « **Reply #23 on:** May 24, 2014, 02:16:40 pm »

Was there any problem with your board BTW or the person speaking chinglish had no idea how to make a board?

rfbroadband · « **Reply #24 on:** May 24, 2014, 03:29:25 pm »

upload your files to EuroCricuits. You will get immediate and detailed feedback from their webpage on DRC errors from their webpage including pictures that incl. markers on the critical errors on your PCB....


EEVblog Main Site	EEVblog on Youtube	EEVblog on Twitter	EEVblog on Facebook	EEVblog on Odysee

Author Topic: PCB Rejected (Read 29363 times)

Share me