Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

I am thinking of using DesignSpark for PCB design and pass the files on for manufacture.

If I want to miss out the soldering part and get the full boards made by a pick and place machine, can I use DesignSpark or are there any other design tools for this?

share|improve this question
It's best to call the fab house doing the work and ask them. If they don't do placement then they probably have someone else and know their requirements. If you want to fab somewhere then build somewhere else you'll need to make sure you meet both PCB fab rules and the pick-and-place requirements by talking with both of them ahead of time. – user6972 Apr 1 '14 at 19:54

Coming from a production facility I can say that we do not require a specific PCB design tool. We (and probably all the other manufacturers) have the tools to convert your files to our required formats.

We would ask you for either Gerber or ODB++ files plus a report (of whatever kind) of Components and Pick'n'Place coordinates (or coordinates just in general). Something like a spreadsheet or CSV with the following columns:


Usually you can simply hand over the data (which is output by DesignSpark or any other tool) and the production facility will take care of your PCB, stocking parts and production (+ what else is needed).

Also, you might want to ask your production facility for a list of components they already have stocked or already available in their system. This has benefits for you and the production facility:

  • You can probably use parts which are stocked or used in large quantities already (cheaper)
  • If you use parts from the company, you can immediately assign their Article number so they won't have to look up the parts, thereby making the process shorter for the producer (and cheaper for you).
share|improve this answer

Any of the commonly used tools should do the job. The key is to have fiducial marks on the board to facilitate the process. Use a 0.1" diam filled circle with no solder mask on it. Try to put at least two in various places on a small board, and more on a large board. I've seen some folks put them only in the scrap parts on a panelized board. Don't do this.

Also, unless there is some reason not to, the assembly houses I've worked with prefer that you give them the Gerbs for ONE BOARD, and let them panelize it for you. They're going to charge you the NRE's anyway, let them earn it.

share|improve this answer
fiducial marks are not always required, best to ask the board house if they need them. And you can sneak some nifty features into panelized designs, such as VCC and GND to all boards for faster and easier in-panel testing of all the boards before breaking out. You will need to use tabs with vias rather than V-grooving though for the most part. – KyranF Mar 31 '14 at 14:25
Yup -- Lots of nifty stuff can be done when panelizing. I like leaving cutouts for things hanging off the sides of boards (for some added cost), like usb connectors, to make them easier to break out, and my assembly house seems to appreciate the effort. I don't see much harm, though, in providing fiducial marks routinely. Nobody makes the pick and place use them! – Scott Seidman Mar 31 '14 at 18:09

If you can afford it, get Altium. Or a student edition or something. PCB manufacturers will take pcbDoc files straight from this. Same with Eagle though as well. Not sure about DesignSpark to be honest, if PCB places use those files directly. Best to ask them, or ask them how to make Gerber files from DesignSpark.

I recently made a panelized design, for design for manufacture. I did not do anything "Special" in terms of placement, just my usual layout techniques and dont clutter your components up too close (leave 1mm or so at the very least! between small passive components like resistors).

The issue I ran into with Altium was my schematic symbols "Comment" fields did not have the exact manufacturer part number from my Bill of Materials on them, so when the PCB assembly guys went to program the Pick and Place machine, the components on the PCBDOC file didn't have nice comment fields as they had expected (nobody told me this, i learned the hard way). Instead I had made a component designator -> manufacturer part number assignment spreadsheet in Microsoft excel which they ended up using to work out what parts went where on the board file.

Altium component positions and orientations are pulled directly out of the file and used for pick and place machine programming. I suspect other PCB CAD programs can generate pick and place files too, but I only know of Altium's capability.

I also made a separate board file and deleted all the components that I did not want loaded, and made PDF documents showing the top and bottom side component layouts in a really nice and obvious fashion for the manufacturers to see what I actually wanted loaded. My design had a lot of extra functionality that I only needed on 10 out of 120 boards, that is why I had spare pads..

I hope this helps?

share|improve this answer
Just a quick sidenote: You do not need to make a separate board in Altium, you can just use Variants and use the generated output files (PnP, BOM Report, Gerber, ...). Also, the way via an extra file is usually the way to go, especially once you have 3 or more variants you probably don't have any other choice. Since the production of the PCB is a major cost factor (especially for lower volumes) you want to have as few as possible different layouts (basically just one). – Tom L. Mar 31 '14 at 11:44
Also, that Comment-thing must be historical. We used to work in that way as well but have switched a while ago because that approach was just .. well .. very limited. – Tom L. Mar 31 '14 at 11:46
I know that the PickNPlace report in Altium only displays the comment field, but you can easily create an identical report through the Bill Of Materials (BoM) report. – Tom L. Mar 31 '14 at 11:53
yeah these guys were old-school. And I only made an alternative (using save-as) PCB file to keep my real design intact. It was just easier for me to create a temporary PCBDOC and delete stuff and all the traces than try to hide things or unlock components/headers I had locked in order to hide them again. I've seen the Variants feature of altium, looks cool but I have not yet tried to use it. I think you are right with the needing to make separate boards anyway. And the BOM manager is great, if you comment every part like I should have (and will from now on!) – KyranF Mar 31 '14 at 11:58
We recently had a project with 13 or 14 variants, the main engineer got crazy when they kept adding variants (although we've been using the Variante feature throughout the project). – Tom L. Mar 31 '14 at 12:03

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

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