Panelization for volume manufacturing: possible?

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Posts: 8
Joined: 06 Dec 2013, 07:38

Panelization for volume manufacturing: possible?

#1 Post by phoenix710 » 25 Jan 2016, 13:27

I've used DipTrace for about a year now and have successfully implemented and built about 100 PCB layouts. Overall, the tool works pretty well, especially at its price-point. (So, I offer my sincere compliments to the DipTrace team.)

The purpose of this note is to discuss some of the issues of panelization.

Others have noted the cost efficiency of combining multiple designs into a single "panel": (PCB Panelization - Tab Routing, ... ion#p16753). There are two main methods: copy/paste, and Panelization.

I have used the copy/paste method myself twice to get four or five different prototypes together with a single setup charge. (Note that not all PCB shops allow this.) Moreover, a few weeks ago, I experimented with the Panelizing option (Edit -> Panelizing...) and it does what it purports to do; for reasons mentioned below (and others not mentioned), I did not submit any Panelized design to a PCB shop.

There is, however, a very real and difficult-to-solve issue with both of these methods: exactly how does one specify a true tab-route panel suitable for use with the automated pick and place machines and reflow ovens? There are two basic layout components needed for this: the tab ("mouse bite") itelf and the route.

On the one hand it is very easy to lay out the tab (this is merely a few ~32 mil holes, typically 5, set back from the board edge a few mils). One the other hand, the problem is the route path itself (which is not so much a layout issue as it is a CAM issue for the 3-axis drill/router in the typical PCB shop).

One approach that I'm now trying is to create a route "layer" in the PCB, then use copy/paste of the PCBs I wish to panelize. (The Panelizing option makes the route "layer" clumsy to implement.) On that "layer" I use a 1.6 mm/63 mil "trace" for the route path (which appears to be the "standard" route channel width). I've submitted a test file set to two different PCB shops to determine whether they can convert the route "layer" into the CAM route commands. (Please note that when generating the Gerber for this layer, ensure that ONLY Trace is checked.)

If this test submission is NOT successful, then the following is moot. However, if the shops tell me that this is workable, then DipTrace users can create volume production panels efficiently according to their own manufacturing rules. Currently, though, this is difficult.

That "difficulty" is the ability to specify the X/Y endpoint coordinates of the "trace" in the route "layer". In order to control the layout of my boards within a panel, I had to set the snap grid to 1 mil to get the needed layout resolution. While possible, this can get unwieldy quickly. It would be MUCH better to lay in the trace to an approximate grid, then "fine tune" the endpoints (mathematically) in a manner similar to editing a line in the assembly layer or the corners of a board outline. As I quickly discovered, there is no way to verify that the route "trace" is EXACTLY where I intend/need it to be. Nevertheless, to ensure the size and position of each PCB is correct, EXACT control is needed. (BTW, attempting to set a snap grid for this is practically impossible, since the boards need to be located according to their size, not a regular layout grid. You literally would have to set the snap grid for EVERY trace segment, one at a time.)

Again, if the PCB shops are able to process the route "traces" into CAM commands, then my strong recommendation to DipTrace is to add the ability to edit trace endpoints. This single, simple feature would move DipTrace into huge usefulness for small businesses (like mine) that is not attainable with EDA packages in this price range.

I'll update this post as I hear back from the PCB shops. If their response is positive, then I hope that the DipTrace team will make this simple request (trace endpoint edit) a priority.

Of course, if anyone has done this successfully, I'd love to hear from you and compare notes.


EDIT 1/26/2016
The first of two PCB shops (Wurth Electronik) has confirmed that the route layer can be read without problem and translated as a route command. So, in principle, this method is workable.

The issue remains of the real limitation within DipTrace of placing the endpoint of a "trace" at a precise, mathematically-constrained X/Y point, rather than on the snap grid. Still researching this; and, again, I'm open to any suggestions.


EDIT 1/28/2016
The second of two PCB shops (PCBWay) has confirmed that the route layer can be read without problem and translated as a route command.

I developed a new method and workflow to create the route "layer" in an efficient way, that maintains the accuracy needed to accurately position the routes. I'll be documenting this with a How To video on my site in the near future. This new workflow is a very effective work-around the limitation of being unable to edit the endpoint(s) of traces (and is probably a better method anyway). (I have a huge block of work ahead, but I'll post as soon as I'm able.)

The SiliconHacker

Posts: 1
Joined: 02 Feb 2017, 11:43

Re: Panelization for volume manufacturing: possible?

#2 Post by patrickh197835 » 03 Feb 2017, 08:04

Hi all

I know its an oldish thread but thought i'd stick my two cent worth in. What I have done to panelise different PCB designs is, do out each design from schematic to PCB separately and generate gerbers. So lets say Board A - D, do full workflow schematic to gerber for each. Now open a new PCB file and IMPORT the gerbers for each board one at a time. Warning however after importing all the necessary files for Board A, select all and move as Board B will import into the same location, so you have to move each board after importing. This has worked well for me so far but still playing about to get best results


Posts: 27
Joined: 20 Apr 2017, 01:33

Re: Panelization for volume manufacturing: possible?

#3 Post by freddy63 » 19 Feb 2019, 09:15

patrickh197835 wrote:
03 Feb 2017, 08:04
Now open a new PCB file and IMPORT the gerbers for each board one at a time.
But copy/paste from PCB should be same result, though way more simple and faster (no need to make GERBER, set all layers etc) or am I wrong?

Anyway for me, trying with GERBER import or direct copy/paste, Diptrace stops working as soon as I paste the second design in the file I'm preparing for panelization. On OS X, 2.5 GHz Intel Core i7 that I use without any issue for 3D, music and video.
I found a workaround by making top and bottom layers invisible, so the software reacts :(

If I have only 1 copper pour in this file that I'd like to use for panelization, than all works, but not if 2 on top and 2 on bottom. I have 2 and 2 cause I want a panel with 2 different deisgns (actually 3, but let's say 2 for now), not an identical replicated. If I needed an identical replicated, I'd use the "panelizing" function under the EDIT menu.
Any idea what is the issue?
Is it because it has more than 500 pins (working at the moment with upgrade version which allows up to 1000 pins)?¨

EDIT: okay. I tried with 300 pins in total and the software does not freeze. It means I have an issue with this larger project.

Post Reply