PCB Layout Guidelines for Pick & Place Assembly - Page 1
Forum section: electronics / general

author: Falcon69
author_rank: Super Contributor
timestamp: January 27, 2015, 04:43:34 am
content: Can we get a sticky about this information?I tried to do a search on Google, and came up with many different layout dimensions regarding this.My question is, what are the minimum, standard, and max (well, max is probably infinite) dimensions or placement:Dead space for PCB Assembly machines to hold onto (the amount of board needed from the edge of PCB to the actually circuit board)Fiducials, I understand that 1mm diameter is minimum, with 3mm diameter of soldermask keepoutDimension from edge of board for fiducialPlacement of fiducial (all four corners, or just the two opposite corners?Width of Route for board separation (i.e. for tab routing), I've been told, from different PCB manufacturers, that they use 1mm bit for this. Dave's video says 2.4mm, which to me sounds pretty bigTABS: what size hole needed and space between centers for breaking apart the boards?Tooling hole size and placement (Dave showed them on his video. They were on the corners of the panel, and fiducials were near them. Are they actually need for the fab house? Or are they their for the end user/customer?Any input on this would be appreciated. I am thinking of having my boards assembled, but, I don't know what manufacturing facility I am going to have do it. I'd like to design the panel for minimal spacing/dimensions to keep the overall size of the board down, which would reduce costs.I was thinking maybe 5mm ends (for machine to hold onto) for the sides with the fiducials on them. 1mm space between the individual boards for routing tabs. 0.3mm holes on 5mm centers for tab routing.Any other things I should plan for when setting up my board for PCB Pick and Place Machines?What about orientation of parts? DO I have to order in the reels, figure out where pin one is on each component, then adjust the text file for the rotation of the parts? How does the PCB program know how the parts are oriented on the reels?When sending in this text file, is there a certain way to label the columns or sort, like, for instance:| Ref. # | X | Y | Z | Orientation | Part # | Value | Package |I'm new to this assembly thing. I just want to save the manufacture from extra work that could cost me.Thanks for your input. A sticky of some sort on these specifications would be great!

author: steve_w
author_rank: Regular Contributor
timestamp: January 27, 2015, 11:52:56 am
content: Good Idea, I second the motion!SW

author: tszaboo
author_rank: Super Contributor
timestamp: January 27, 2015, 12:10:13 pm
content: Most of these questions are answered by IPC-2221. I think it is something worth having if you design boards in bigger quantities. About the second half of your questions, I recommend reading Tom Hausherr's blog at mentor graphics, it is probably the most professional and complete guide you will find for it.http://blogs.mentor.com/tom-hausherr/

author: Falcon69
author_rank: Super Contributor
timestamp: January 27, 2015, 07:07:51 pm
content: thank you NANDBlogI will design the board with those specs.It said for 0.65 pin pitch placement, use 0.5mm grid and 1.0mm grid for the vias. I've stayed with the default 0.159mm for both. So I'm hoping that will be okay. I do not want to redo everything. I've left enough space between pads and vias, of course.

author: Falcon69
author_rank: Super Contributor
timestamp: January 28, 2015, 10:56:52 pm
content: i sent a blank pcb board design with my tabs/holes, tooling marks, fiducials, and routing to Elecrow. Hope to get a response soon before running traces and placing pads. According to Elecrow's wiki site, they use a 0.8mm bit for the routing, and minimum routing width is 1mm. So my route tabs at 1mm wide should be okay. I will let you all know what they say.

author: EEVblog
author_rank: Unknown
timestamp: January 28, 2015, 11:26:48 pm
content: Quote from: Falcon69 on January 27, 2015, 04:43:34 amDon't fuss over this, your assembler will do all this for you and double check everything and almost certainly change stuff anyway into whatever format is required for the machine and software they use.This is all included in the setup cost for the pick and place machine. The people that do this are very quick and efficient, and generally a low wage, so it's not costing you enough to worry about any of it. A couple of one-off hours of labour for a smallish board probably, maybe a day for larger board.Your PCB program does not know nor care how the parts are rotated, or where the center of the component is, apart from alignment during placement before routing.QuoteJust send them whatever format your PCB program outputs and let them worry about it.

author: EEVblog
author_rank: Unknown
timestamp: January 28, 2015, 11:29:58 pm
content: Quote from: Falcon69 on January 27, 2015, 04:43:34 am2.4mm is a standard routing bit size for board outlines etc, it allows them to go faster and route more stacked boards at once without snapping bits.So if you have the space, specify a bigger routing path to make use of that bit.Yes, they can certainly use smaller routing bits if needed. But the smaller the bit gets, the less boards can be routed at once, and the slower the bit has to travel which equals more time and technically most cost. But for the boards you are talking about, don't worry about it.

author: Falcon69
author_rank: Super Contributor
timestamp: January 28, 2015, 11:36:41 pm
content: okay, thanks DAVE. that makes sense abit the bits snapping. but, i want to try and keep 3 sets of pcb's on a single size A4. So I am stuck using a 1mm spacing on the routing outs. What are general sizes for a pcb to be assembled? you mentioned on your video A4 size, are there smaller sizes as well that work okay? Must the tooling rails be 10mm or can they be smaller?

author: IconicPCB
author_rank: Super Contributor
timestamp: January 30, 2015, 05:20:08 am
content: I run a small pick and place machine. No need for tooling rails as the machine can handle single routed boards.Talk to Your assembly house and follow their instructions. General size of PCB is what ever the particular assembly house can do.I have processed single board which are approx 300 x 400mm no tooling rails.

author: EEVblog
author_rank: Unknown
timestamp: January 30, 2015, 06:01:04 am
content: Quote from: IconicPCB on January 30, 2015, 05:20:08 amSingle routed boards generally require a custom holder for automated movement along the machine (from stencil, to PnP, to oven).Unless you absolutely have no other choice, put tooling strips on!

author: EEVblog
author_rank: Unknown
timestamp: January 30, 2015, 06:02:19 am
content: Quote from: Falcon69 on January 28, 2015, 11:36:41 pmTalk to your assembler. Generally the limit is the height, because the conveyor is only a maximum width, Other than that the board can generally be any length.

author: IconicPCB
author_rank: Super Contributor
timestamp: January 30, 2015, 08:18:34 am
content: Dave,You forgot to comment on the final part of the message which reads:"... Talk to Your assembly house and follow their instructions. ..."OK

author: tszaboo
author_rank: Super Contributor
timestamp: January 30, 2015, 10:09:01 am
content: Quote from: IconicPCB on January 30, 2015, 05:20:08 amAlso, if you make single boards without rails, just make sure you are not placing anything 3mm from the edge.For the board routing, my manufacturers are using 2mm and 1mm milling as default, not 2.4mm. I'm sure that in the US it will be like 2.54mm and yet another size if you ask someone else. So best thing to do is ask the manufacturer indeed.

author: Falcon69
author_rank: Super Contributor
timestamp: January 30, 2015, 04:50:01 pm
content: I will probably have Elecrow do it with their 'Premium Service'. I'm tired of trying the offbrand manufacturers (i.e. eBay middle man), there is always something wrong with the board (i.e. misaligned soldermask, off-center holes, nasty looking silk screen, etc.). Elecrow's wiki site says they use a 0.8mm bit to do the routing, and minimum route holes need to be no less than 1mm.There site says NOTHING about the dimensions of the tooling holes or rails however. So far, that eMail I sent them a couple days ago, have gone unanswered.

author: IconicPCB
author_rank: Super Contributor
timestamp: January 30, 2015, 09:47:03 pm
content: Tooling holes and rails.. feducial marks are up to you to implement in line with the assembly house requirement.

author: Zeyneb
author_rank: Regular Contributor
timestamp: February 04, 2015, 09:55:16 pm
content: Quote from: NANDBlog on January 27, 2015, 12:10:13 pmMaybe a bit off-topic but here a bit of a warning:Tom Hausherr is currently working for PCB Libraries. Actually it might be his own company. Much has changed since the last blog of him at Mentor Graphics. Please do not buy LP Wizard if it still exists. I don't think Mentor has knowledgeable people to continue to support this software. At PCB Libraries they have an active forum about subjects like this and IPC standards are changing. Their PCB Library Expert product is constantly adapted to these new changes. The forum has also some links to newer versions of the documents found on the Mentor blogs.

author: free_electron
author_rank: Super Contributor
timestamp: February 05, 2015, 12:59:49 am
content: the short :for single boards without guidance rails- no SMD parts closer than 5mm from the edge- provide tooling holes , typical 2.5mm holes , opposite corners- place a fiducial at the bottom left corner of the board , 5mm inwards from the edge. In your cad tool : set the boards origin to that point so that all pick and place data is generated in respect to this fiducial- place a fiducial top left and bottom right so you get an L shape with 90 degree angle. this allows the machine to compansate for rotational offset.- fiducial is a 1 mm diameter roudn or 1mm edge width square , bare copper with soldermask removed 2mm around it. this is done for contrast reasons. soldermask can be very shiny and reflects light from the camera. removing the soldermask creates good contrast.for boards that are panelized and will be removed using v-scoring or mousebites.- parts can go down to 1mm from the board edge.- fiducials can be on the board frame- parts must be kept away from mousebites at least 3 mm- having anything larger than an 0805 adjacent to scoring lines or mousebites is a no-no as these parts will crack during depanelisation.

author: JuKu
author_rank: Frequent Contributor
timestamp: February 08, 2015, 10:38:31 pm
content: Still, talk to your manufacturer. Free_electron gives good guidelines, but they are not universal. For example, my machine differs slightly:- Origin default location is in the bottom left corner of the board. This is not a big deal, it can be set anywhere (for any manufacturer I know of), but the manufacturer needs to know where it is. I selected the board corner because both of the factories I have been worked with most of my stuff asked origin to there. I have no idea how universal that might be or how universal it is to put the origin at a fiducial.- The algorithm my program uses does not much care where the fiducials are. They don't need to be in certain angels or certain locations. that algorithm needs at least three, four or more is preferred. With three, the accuracy placement suffers outside the triangle. if there are more than four, the accuracy in theory increases. In practice, the transform estimate with four fiducials already gets well below the mechanical tolerances.

author: free_electron
author_rank: Super Contributor
timestamp: February 09, 2015, 06:59:25 am
content: Quote from: JuKu on February 08, 2015, 10:38:31 pm

author: JuKu
author_rank: Frequent Contributor
timestamp: February 09, 2015, 07:01:52 pm
content: Oh, my machine (like any other p&p) uses fiducials for alignment. The origin is just a reference. Of course the macine zero is different to the board zero; further, machine x axis is not board x axis (rotation in board placement); board x-mm is different from machine x-mm (scale error) and same for y axis. These are usually significant (rotation is always). In theory, board 90 degrees is different from machine 90 degrees (shear error, a square is slightly diamond shape on both coordinate spaces, and different). A p&p machine (mine and others) uses optics to measure the location of fiducials in machine coordinates and more or less sophisticated math to transform board (CAD) coordinates to machine coordinates.using board edge as the (default) origin only allows the machine automatically know where to go look for fiducials. If the origin is on a fiducial, you need to tell the machine where in machine coordinates that is. Not a big deal, but unnecessary.Any manufacturer can handle board origin pretty much anywhere, and every manufacturer (at least any that I have worked with) want an explicit mention where it is to avoid costly misunderstandings. My remark of having it at the board corner was just that my fafourite manufacturers like it there, because it saves one (small) step in setup. It does, so I followed.

author: free_electron
author_rank: Super Contributor
timestamp: February 09, 2015, 10:14:22 pm
content: Ah, ok . Got it . The people indeal with want the origin to be on a fiducial. They mentioned something about having boards in panels. Apparently their machines can scan and replicate the placeemnt array automatically (juki and siplace machines mainly)

author: JuKu
author_rank: Frequent Contributor
timestamp: February 10, 2015, 04:38:53 am
content: That makes sense, too. The lesson (as said many times): ask the people doing the work how they like the work to be set up. (Works other areas of life, too.)