PCB Rejected - Page 1
Forum section: electronics / general

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 02:24:23 pm
content: 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.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 02:55:43 pm
content: 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

author: ConKbot
author_rank: Super Contributor
timestamp: May 23, 2014, 02:57:49 pm
content: 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 anotherVias: 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 :pAlso, 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.

author: c4757p
author_rank: Super Contributor
timestamp: May 23, 2014, 02:58:53 pm
content: Did you actually check theGerbers? There are a lot of options when generating them. You should always open and inspect them in a separate Gerber viewer.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 03:12:10 pm
content: 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.

author: c4757p
author_rank: Super Contributor
timestamp: May 23, 2014, 03:16:01 pm
content: Quote from: snipersquad100 on May 23, 2014, 03:12:10 pmYou can just load them into any old Gerber viewer.There are a few online.This oneworks nicely.This oneshould 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 alsothis one.Then there's gerbv, part of gEDA, and KiCad has GerbView. Eagle probably has a viewer as well.ZofzPCBis 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.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 03:18:41 pm
content: Thank you c4757p, I will have a look.cheers

author: mamalala
author_rank: Unknown
timestamp: May 23, 2014, 03:31:49 pm
content: 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

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 03:39:22 pm
content: Cant upload that type of file to this forum.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 03:43:18 pm
content: let me try this.

author: Dago
author_rank: Frequent Contributor
timestamp: May 23, 2014, 03:53:45 pm
content: Gerbv is also a decent viewer.http://gerbv.sourceforge.net/

author: zapta
author_rank: Super Contributor
timestamp: May 23, 2014, 03:55:35 pm
content: You can upload your eagle.brd file tohttp://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).

author: kc0ngu
author_rank: Contributor
timestamp: May 23, 2014, 03:57:49 pm
content: 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

author: nctnico
author_rank: Super Contributor
timestamp: May 23, 2014, 04:09:07 pm
content: 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.

author: mamalala
author_rank: Unknown
timestamp: May 23, 2014, 04:14:10 pm
content: Quote from: snipersquad100 on May 23, 2014, 03:43:18 pmOK, 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 themOn 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

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 05:24:40 pm
content: Thank you for your comments, I will redo the board and let you know what happens.

author: tszaboo
author_rank: Super Contributor
timestamp: May 23, 2014, 05:49:57 pm
content: 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.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 06:23:01 pm
content: thanks nandblog

author: Kjelt
author_rank: Super Contributor
timestamp: May 23, 2014, 09:46:53 pm
content: Also if it is a load and the fets will be used in linear operation do you want to cool them? Just a thought.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 23, 2014, 10:01:38 pm
content: Hence the fets are lind up with mounting holes for the heatsink.

author: Rory
author_rank: Frequent Contributor
timestamp: May 24, 2014, 01:13:57 am
content: 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.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 24, 2014, 10:27:58 am
content: Just found someone to manufacture my boardwww.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.

author: tom66
author_rank: Super Contributor
timestamp: May 24, 2014, 10:33:06 am
content: 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.

author: tszaboo
author_rank: Super Contributor
timestamp: May 24, 2014, 02:16:40 pm
content: Was there any problem with your board BTW or the person speaking chinglish had no idea how to make a board?

author: rfbroadband
author_rank: Unknown
timestamp: May 24, 2014, 03:29:25 pm
content: 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....

author: bithead9
author_rank: Contributor
timestamp: May 24, 2014, 09:47:02 pm
content: Did you try ASKing why they rejected the design ? I got to believe they would tell you. Good luck and let us know what happens!

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 25, 2014, 11:22:14 am
content: @ bithead9 They said there was to much empty space on the board and I should lay it out better.@ rfbroadband Eurcircuits were expensive.@ Nandblog No faults came up on the check.

author: bithead9
author_rank: Contributor
timestamp: May 25, 2014, 04:49:18 pm
content: I guess you tried these guys:http://expresspcb.com/for $51.00 not bad... Not sure of your budget or where you are shipping, etc.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 25, 2014, 09:58:51 pm
content: Quote from: snipersquad100 on May 25, 2014, 11:22:14 amNow I've heard everything.

author: bithead9
author_rank: Contributor
timestamp: May 26, 2014, 01:50:00 am
content: John I agree that is good. Like who are THEY to say your board has too much space??? Maybe I want more empty space for SOME reason. how would they know and why would they even CARE ? Guess they did not need the money ? Strange.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 26, 2014, 02:31:45 am
content: To be fair, and without really analyzing it, the layout and routing is pretty awful and could be a LOT better, but so what? If the rules check passes, just build the damn thing. Learning how to design boards is a process, and it takes time and experience to learn, but that doesn't mean that sub-optimal boards are inadequate. The board is probably fine.How bizarre.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 28, 2014, 07:59:34 am
content: Can someone please help, The board files I sent off to smart-prototyping have sent me the following email:-The comments for your order are:Hello DavidThis is Minnie from Smart-Prototyping Team, thanks for your order.You Gerber file has no outline, please modify it and send me the new Gerber file, thanks.Best regardsMinnieWhat does it mean by no outline? All the layers were active when I created the gerbers.I don't understand.

author: Neverther
author_rank: Regular Contributor
timestamp: May 28, 2014, 08:38:05 am
content: I usually include board outline on silkscreen with couple measurements for chinese prototype services.Gives them the pcb edges without mechanical/pcb edge layer as they do their own panelizing for prototype runs.They cant just assume for example copper pours (+ tolerance if you dont wish to have copper to the edge, they dont know that) as pcb edges, they need you to specify it.I think atleast on chinese sites the description mentions they need the pcb edge alteast on one layer, but dont specify which.EDIT:Looked their site and they give: xxx.GML Outline, so basically you can give them PCB Edge layer/whatever.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 28, 2014, 08:45:11 am
content: Thank you, I will create the dimension on the silkscreen cheers.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 28, 2014, 08:53:16 am
content: The dimension was already on the silkscreen. Im still confused.com

author: 8086
author_rank: Super Contributor
timestamp: May 28, 2014, 09:11:06 am
content: Maybe they want outline on all layers?

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 28, 2014, 09:14:50 am
content: How do you do that then?

author: amyk
author_rank: Super Contributor
timestamp: May 28, 2014, 01:04:33 pm
content: When you get rejected twice by two different services, I think it's safe to assume the problem is your design.Maybe "too much space" is what they tried to say about having no outline but the meaning got lost in translation.

author: Neverther
author_rank: Regular Contributor
timestamp: May 28, 2014, 01:46:55 pm
content: As I previously said: xxx.GML outline layer on their description.I got measurements on silkscreen and on the order I tell the outline is on silkscreen with measurements, but as I said, those chinese dont take outline or mechanical layer on cheapest prototypes.Smart does offer panelizing/routing/grooving multiple designs from one gerber, hence the outline layer.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 29, 2014, 12:54:52 am
content: It's times like this I'm glad I use a service like Sunstone. 100% reliable, headache free, on time every time, and great communication/technical support. I couldn't be happier.

author: HackedFridgeMagnet
author_rank: Super Contributor
timestamp: May 29, 2014, 01:06:53 am
content: Can you post the gerbers? As a zip file you should be able to upload.

author: nctnico
author_rank: Super Contributor
timestamp: May 29, 2014, 01:33:20 am
content: Quote from: snipersquad100 on May 28, 2014, 08:45:11 amA better method is to add an extra fabrication or milling layer which contains the outline of the PCB. A PCB doesn't have to have a rectangular shape BTW.

author: gxti
author_rank: Frequent Contributor
timestamp: May 29, 2014, 02:11:40 am
content: An outline layer should be a separate Gerber file with lines where the edge of the PCB is. If your PCB is a rectangle, that means just a rectangle. No dimensions or comments. How you actually accomplish that depends on the PCB package, usually there's one or more "mechanical" layers you can use for any purpose. Choose one as your outline layer and mark the file as such (by renaming it, for example) when you send it off to be manufactured. Some packages have a builtin idea of "board shape" and can export it to a gerber file automatically if you tell it to.As a pre-flight check you can always upload a zip of your gerber files tohttp://gerblook.organd it will preview how it looks. It also makes sure you've got all the right files inside before you send it off to be manufactured.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 29, 2014, 12:02:49 pm
content: I cant upload the zipped files as its over 1000kb sorry, if anyone wants a look I can e-mail them to you.

author: zapta
author_rank: Super Contributor
timestamp: May 29, 2014, 01:32:04 pm
content: Quote from: snipersquad100 on May 29, 2014, 12:02:49 pmDropbox is good for things like that. You put the fine in you Dropbox directory and share a link to the directory or file.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 29, 2014, 03:36:13 pm
content: This is the link to the zip files.https://app.box.com/s/u0ypx78iga72hokwmyi3

author: Neverther
author_rank: Regular Contributor
timestamp: May 29, 2014, 06:09:13 pm
content: File extensions are all different when compared to what smart-prototyping wants.Maybe they cant tell which is board outline layer.No front copper?What is "J**.cmp"? Seems like combination of *.plc (front silkscreen) and *pls (edge with measurements drawn into it?).(No Eagle here so cant check)

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 30, 2014, 08:28:16 am
content: LIst of layers with file typs for eagle.Component side .cmpSolderside .solSilkscreen CMP .plcSilkscreen SOL .plsSolder stop mask CMP .stcSolder stop mask SOL .stsGenerate drill data .drd

author: Neverther
author_rank: Regular Contributor
timestamp: May 30, 2014, 03:08:44 pm
content: I hope this isn't what you sent smart-prototyping as front copper:

author: daveshah
author_rank: Unknown
timestamp: May 30, 2014, 03:24:52 pm
content: I have generated what I believe to be a correct set of gerbers using Smart Prototyping's CAM file - but I accept no responsibility for them.https://www.dropbox.com/s/q6wyrstjpd7b3se/Dummy%20Load.zip

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 30, 2014, 03:29:04 pm
content: I don't know what im doing lol, I just put all the layers of and generate the gerbers using spark fun electronics gerber tool. I sent them some files but they said there were no dimensions so I added them and resent them, I put them on several layers so they don't miss em lol.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 30, 2014, 03:30:58 pm
content: Thanks daveshah, I will send them now. Last I hered from them is that everthing is fine but I will still send them.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 30, 2014, 05:54:10 pm
content: Hi daveshah, How have you got different file extensions than mine then?

author: daveshah
author_rank: Unknown
timestamp: May 30, 2014, 07:53:46 pm
content: I generated those gerbers using Eagle 6.4.0 and the CAM file off Smart Prototyping's website (http://smart-prototyping.com/image/data/1_services/1_electrical/100201%20-%20Eagle%20Design%20Rules%20and%20CAM.zip)

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 30, 2014, 10:04:37 pm
content: Thanks daveshah

author: kc0ngu
author_rank: Contributor
timestamp: May 31, 2014, 04:10:59 am
content: The board house in requesting an outline is looking for a gerber with the extension .GKOTo generate this in Eagle draw a watertight line around your pcb design. Select the wire tool and then make sure the diimension layer is active (layer 20 in Eagle). Draw a watertight line around the board. When you fire up the CAM processor make sure that an outline tab is available, in file it will be outputting the file with extension .GKOWithout this gerber layer most production houses will reject your design.Hope that helps.Jeremy Blum has a great series on designing your pcb for manufacture including in Part 3 how to output a CAM job. Search You Tube for him and that series.Good Luck

author: snipersquad100
author_rank: Frequent Contributor
timestamp: May 31, 2014, 07:49:02 am
content: Thanks kc0ngu for the advice.I've been following the guys tutorials on youtube.

author: LukeW
author_rank: Frequent Contributor
timestamp: May 31, 2014, 11:59:04 am
content: Don't use weird extensions like .sts or .cmp.Set up the CAM processor to use standard extensions to identify the different layers in the gerber files, such as .GBO, .GTS etc and .TXT for the drills.

author: amyk
author_rank: Super Contributor
timestamp: May 31, 2014, 12:26:44 pm
content: Quote from: Neverther on May 30, 2014, 03:08:44 pmImagine the results if someone swapped the silkscreen and copper layers and the fab let that through...

author: nctnico
author_rank: Super Contributor
timestamp: May 31, 2014, 01:57:56 pm
content: Quote from: LukeW on May 31, 2014, 11:59:04 amWho said that is standard? Just use the standard extensions for the PCB package. The PCB makers are smart enough to work out what package you are using and figure out which layer is which.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 31, 2014, 04:49:00 pm
content: Again, Sunstone has this one right. You upload the files, and then select which file is which layers. You can name them whatever you want, and there's never any ambiguity.

author: signality
author_rank: Newbie
timestamp: June 02, 2014, 10:20:07 am
content: Quote from: snipersquad100 on May 23, 2014, 02:24:23 pmIt's a pity you didn't get a more helpful response from EasyEDA but some of that may have got lost in translation.Just a thought but what I would suggest is that - given that you admit to being a novice at PCB design - you might like to try just doing a very simple design right the way through to PCB Gerber generation and checking, using EasyEDA but following this How To article:http://www.edn.com/design/pc-board/4430173/2/EasyEDA--Free-online-EDA---Product-how-toAssisted if necessary by their tutorial:http://easyeda.com/EasyEDAtutorial/.That will show you what a complete, finished set of Gerbers will look like.Then you could try importing your Eagle layout into EasyEDA to do some further processing to get it so that you can submit a set of Gerbers that look to have all the same sort of layer files (though your PCB may have more : I don't know how many layers yours is) and features, such as board outline, as the simple demo project.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 02, 2014, 09:51:02 pm
content: Ive tried submitting a few designs to different board manufactures but they all come up as "I can't find a board outline file"How do you make a board outline file using eagle??? Do I need a certain cam job file or do I make it in the pcb layout.

author: mamalala
author_rank: Unknown
timestamp: June 02, 2014, 10:55:09 pm
content: Quote from: snipersquad100 on June 02, 2014, 09:51:02 pmDid you read the posts that have been made? FFS, at least i have written where the outline goes in Eagle. Its the layer called "Dimension", layer 20.Either generate a separate file with only that layer active, or have that layer active in _every_ file you generate. That is, top/bottom copper, mask, silkscreen, etc. The latter is a method that pretty much everyone can handle, because it's easy to see that there is the same outline in every single gerber file, so it must be the board outline.Also as mentioned, make sure to check the "pos.coord" tickbox in the cam, for every file you export, as this will align all the files to a common coordinate point. This is _especially_ important if the outline is in only one file and nowhere else...Geez... What is so hard with reading, or looking at (let alone using) cam files provided by the manufacturers...Greetings,Chris

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 02, 2014, 11:50:55 pm
content: haha, I read that post,but it still wasn't working. However I figgered it out, I don't know why but on layer 20 the dimension the boarder was visable but I had to use the wire tool to redraw the boarder. I don't understand why I had to do that as the boarder was visible. Maybe ive disabled the boarder in the settings or something.Anyway it seems to be working now, thanks for the help.

author: mamalala
author_rank: Unknown
timestamp: June 03, 2014, 01:38:33 am
content: Quote from: snipersquad100 on June 02, 2014, 11:50:55 pmIf you had something visible somewhere, but no outline on layer 20, then it wasn't the dimension layer at all.Like you drawing all the parts outlines on some layer that has nothing to do with in the first place.In any case, typical case of PEBKAC.Greetings,Chris

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 03, 2014, 08:08:26 am
content: I wont ask what PEBKAC stands for.

author: amyk
author_rank: Super Contributor
timestamp: June 03, 2014, 12:29:23 pm
content: Quote from: snipersquad100 on June 02, 2014, 11:50:55 pmWait until after you get the boards back before you proclaim success...

author: LukeW
author_rank: Frequent Contributor
timestamp: June 03, 2014, 02:06:20 pm
content: Quote from: nctnico on May 31, 2014, 01:57:56 pmGerbers that are provided for PCB fab and their acceptance by the fab house to fab the boards should be completely independent of "what package you are using", the fab house doesn't want to or need to know.

author: SirNick
author_rank: Frequent Contributor
timestamp: June 03, 2014, 07:22:20 pm
content: Maybe the OP would have better luck with a more user-friendly package? Eagle is crap, IMO. There's always a learning curve for CAD software, but "learning curve" is completely different from "brain-dead UI".OP: Give Robot Room's Copper Connection a try. It's a surprisingly useful little PCB design tool. Just as friendly as ExpressPCB, but it isn't vendor-locked and can output straight to Gerber.

author: senso
author_rank: Frequent Contributor
timestamp: June 03, 2014, 07:36:04 pm
content: Just grab the CAM file from seeedStudio, and use it, and also remenber to NEVER save changes after running the CAM/Job, done, whats so hard about that?

author: zapta
author_rank: Super Contributor
timestamp: June 04, 2014, 05:24:48 am
content: Quote from: senso on June 03, 2014, 07:36:04 pmWhy?

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 04, 2014, 07:24:11 am
content: Because if you don't know what your doing "like me lol" you end up saving the cam job after you've made changes by mistake.I learned that lesson the hard way.I think I got the grasp of it now.

author: zapta
author_rank: Super Contributor
timestamp: June 04, 2014, 07:55:56 am
content: Quote from: snipersquad100 on June 04, 2014, 07:24:11 amI see, I thought the concern was that the cam job changes the schematic or board layout.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 04, 2014, 08:20:52 am
content: No, I believe that if you add or take away layers from the cam job and you don't know what your doing and them save the changes you will mess up that cam job. On the other hand if you know what your doing then saving isn't a problem.Im sure I will be corrected by a boff if what im saying is wrong lol

author: miguelvp
author_rank: Super Contributor
timestamp: June 04, 2014, 09:00:25 am
content: You can always take a cam job and save it as a WIP (work in progress) so you can always go back to the original, you could add versions to it too so you have a history of changes.

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 04, 2014, 09:48:45 am
content: I have write that down, thanks

author: snipersquad100
author_rank: Frequent Contributor
timestamp: June 17, 2014, 06:53:45 pm
content: Hello again.My pcb's arrived today, I said I show them when they come so here they are. They took a few weeks to come but for the price I cant grumble. I will defo use smart prototyping again, and now I've got this gerber business sorted I be doing more projects this way.