"IT'S TOO BIG!" says everyone, including my PCB assembler...

[frogblender]

I have a motherboard which clocks in at a very impressive 33" x 17".

Indeed.

Getting the raw card built is no problem.  But the smt shop, and the few other smt shops I spoke to,  all say it is too big - it won't fit in the smt machine, won't fit into x-ray, won't fit into the reflow oven, and just plain won't fit.  Anywhere.

I hate when that happens.

Anyhoo... I want to cut it in half, and slap in some connectors and whatnot to jumper the nets and power that got cut (there aren't that many nets that cross where I want to put the cut line), and then the smtShop can build each half individually.   The smtShop will be supplied with the two raw cards, two boms, and two placement files. 

But... in altium, I don't want to have two separate designs.   I have the great big design already done, including the 33x17" pcbDoc, and I've drawn the line where it'll be cut.  So the question:

In Altium:  from a single pcbDoc:  how do I generate two sets of gerber, two boms, and two placement files?

[james_s]

Wow, can you share what this is? I haven't seen a board that big since the old days of TTL, seems like I saw a CNC machine controller that had a board about that size but even that I'm not sure was quite THAT big.

[thm_w]

Don't think this is the best way but:
- delete left half of the board, generate gerbers
- undo, delete right half of the board, generate gerbers

BOM I'm sure you could select the parts on the PCB, cross select that on the schematic, and maybe change a property/variant to left/right then generate BOM for each.

[I wanted a rude username]

33" x 17"

840 x 430 mm

I'm not sure the FR-4 even comes in such a length ... and among the other problems already mentioned, layer alignment is going to be difficult on that scale.

Might be worth taking a step back and asking, is this actually the right solution? Could a modular design be more suitable? What about the backplane-and-modules architecture, in use for over half a century in big iron like today's blade servers?

[mikeselectricstuff]

If it will be made as two boards I don't think it makes sense to keep it as one design file, as any changes mean you'll need to go through the process of splitting again.

[mikeselectricstuff]

33" x 17"

840 x 430 mm

I'm not sure the FR-4 even comes in such a length ... and among the other problems already mentioned, layer alignment is going to be difficult on that scale.

PCBWay will quote for up to 1200x1200mm I've done up to about 1.5m long, but found the hard way that material availability becomes very problematic over 1.2m, especially if you want less than 1.6mm thick!
I know one assembly house in the UK that can do up to 1.6m long, but only about 350mm wide.

 

[Kean]

I don't think splitting the gerbers would be too hard to manage, even if it may involve manual post-processing.

As suggested by thm_w, I think the best way to handle BOM and PnP files is using variants to split the two halves.
For one variant/half you would need to adjust the origin, or manually offset all the co-ordinates.

[ajb]

If you want this design to be maintainable then I think the best approach is to make two copies of the whole project, delete everything on one side form one and on the other side from the other, and then just have a left and a right project. You could then add both boards to a multi board project, which won't be the same as having one PcbDoc but maybe better than having fully independent projects?  All of this reworking of the design will likely be easier if you design the connectors in first.

If you just want to get it done once, then thm_w's suggestion is probably the way to go except that I don't know if you can easily set a whole bunch of components as not fitted in a variant in one go. Every time I've done that it's been a lot of clicking on every single part, but maybe there's a better way I don't know about.  It might be easier to post process the PnP file to filter out components by their coordinates? Depends on how many components you have, I guess.  If you can get the part coordinates into the BOM (I would imagine that's possible, but don't know for sure) then you can do the same thing there.

[ANTALIFE]

As others have said, ideally this would be two (or more) projects...

If you are bent on keeping it as a single project (with a single PCB file) then you will need to make sure there are no repeated designators and that the broken connection errors the DRC throws up make sense. Then generate the Gerber, NC Drills, P&P as usual and make it really clear which board is which. Give all files to your PCB fab/assembly house and tell them something like, I want 2 copies of board Y and 4 copies of board X. They will be able to separate the two designs when they generate the machine file, though they would probably charge you a bit more as there is more work involved in doing so. If this sounds like a lot of steps to worry about then time to split up the single project...

[frogblender]

As others have said, ideally this would be two (or more) projects...

If you are bent on keeping it as a single project (with a single PCB file) then you will need to make sure there are no repeated designators and that the broken connection errors the DRC throws up make sense. Then generate the Gerber, NC Drills, P&P as usual and make it really clear which board is which. Give all files to your PCB fab/assembly house and tell them something like, I want 2 copies of board Y and 4 copies of board X. They will be able to separate the two designs when they generate the machine file, though they would probably charge you a bit more as there is more work involved in doing so. If this sounds like a lot of steps to worry about then time to split up the single project...

If it will be made as two boards I don't think it makes sense to keep it as one design file, as any changes mean you'll need to go through the process of splitting again.

The though of splitting it in two separate project gives me chills:  the design is heavily heirarchical, and splitting all that up, figuring out what bits go on which half, and hoping you don't miss anything... and then deleting the other half.. and hoping you don't delete too much... and all the dangling nets that are likely to result... all that all seems like a nightmare. 

Currently, as a single design, the gerbers are perfect:  there is one gerber output, with a cut line down the middle;  I could just give it to the boardshop as-is, and get two raw cards in return.
As for assembling the board:  I cooked up a .net, which takes the single pick-n-place file, parses each line, and if the x-coordinate of a component is on the left of the cut line, it writes the component to  PNP_LEFT.txt,  otherwise it writes to PNP_RIGHT.txt.   Works a treat. 

The next logical (and so far incomplete) step is to use the LEFT and RIGHT pnp files to similarly split up the bom.csv into bom_LEFT.csv and bom_RIGHT.csv.

It is a post-altium step to run the .net utility, but it is a single command that executes in a second.

If anyone can see any flaws in my methodology, please let me know.

[mikeselectricstuff]

Not familiar with Altium but I use PCAD2006 which I believe has some similarities. Could you not drag-select all components on each side in turn and set their value property to "NF"

[Just_another_Dave]

Although I’ve never used it, Altium provides tools for designing multiboard projects (including mechanical collision detection). Maybe it isn’t too difficult to divide your design into 2 PCBs while keeping a single schematic

[tszaboo]

As others have said, ideally this would be two (or more) projects...

If you are bent on keeping it as a single project (with a single PCB file) then you will need to make sure there are no repeated designators and that the broken connection errors the DRC throws up make sense. Then generate the Gerber, NC Drills, P&P as usual and make it really clear which board is which. Give all files to your PCB fab/assembly house and tell them something like, I want 2 copies of board Y and 4 copies of board X. They will be able to separate the two designs when they generate the machine file, though they would probably charge you a bit more as there is more work involved in doing so. If this sounds like a lot of steps to worry about then time to split up the single project...

If it will be made as two boards I don't think it makes sense to keep it as one design file, as any changes mean you'll need to go through the process of splitting again.

The though of splitting it in two separate project gives me chills:  the design is heavily heirarchical, and splitting all that up, figuring out what bits go on which half, and hoping you don't miss anything... and then deleting the other half.. and hoping you don't delete too much... and all the dangling nets that are likely to result... all that all seems like a nightmare. 

Currently, as a single design, the gerbers are perfect:  there is one gerber output, with a cut line down the middle;  I could just give it to the boardshop as-is, and get two raw cards in return.
As for assembling the board:  I cooked up a .net, which takes the single pick-n-place file, parses each line, and if the x-coordinate of a component is on the left of the cut line, it writes the component to  PNP_LEFT.txt,  otherwise it writes to PNP_RIGHT.txt.   Works a treat. 

The next logical (and so far incomplete) step is to use the LEFT and RIGHT pnp files to similarly split up the bom.csv into bom_LEFT.csv and bom_RIGHT.csv.

It is a post-altium step to run the .net utility, but it is a single command that executes in a second.

If anyone can see any flaws in my methodology, please let me know.

One project, one PCB, that's how it works.
You can put them into a project group, which might give you an advantage. IDK what, it is a relatively new feature.

[epongenoir]

Have you tried with circuit variants? Once I stumbled into a Webinar about them, and it might be fitting at least for the BOM

[free_electron]

i call BS. You cannot simply cut a layout in half and then 'wire it using connector'. where are those 'connectors' in your design ? How do you assign signals ? if you cut the board : the trace stubs are still covered in soldermask . How will you solder that ?
There is much more going on here than simply 'cutting a board in half'

[AJbotic]

Add your connectors, breaking the nets that cross your intended division.  Put a massive slot/cutout in at the division.  Generate your gerbers.  Edit the artwork in CAM to have 2 sets, or ask your chosen manufacturer to do it for you. Once the nets are broken and slot is there, these are easy operations in CAM.

[frogblender]

Thanks to all who replied (even the guy who called "B.S.").  Just to keep yous all up to date: 

I kept it as one big single project.   I generated one set of gerbers, gave a dimensioned drawing showing my cut line to the boardshop, and their Gerber Jockeys split the gerber into two.    My home-brew .net code takes the one pick&place, and splits it into two, and then splits the bom into two.
The boards are currently being fabbed, and the smt shop has their feeders fully cocked and loaded; both are reporting no issues.

Boardshop gerberJockeys spend all day cutting/pasting/rotating gerbers, squeezing all kinds of designs to maximize panellization... so I think this was trivial for them.  I could've done it with viewmate or something... but better to let them do it.

Keeping it as a single project in Altium was the way to go.   The big drawback is the monstrously large (300MB?) single boardfile, which takes altium 10 friggin minutes to even open the dang thing.   But it is convenient to have the whole board, schematic and layout, all in one design.


As an aside:  For fun, we fabbed the original 33x17", at full size, no cuts.  I have a raw card in hand; it is big... in a pinch, you could use it as a ping-pong table, or perhaps foozball.  They haven't gone through SMT yet...  we had to find a smtShop  that could handle this size.   It is heavy and sags and bends just by picking it up.  Not sure if it'll be better or worse once ~10 kilograms of components and connectors are plopped on it. 

[Daixiwen]

Pictures or it didn't happen

Seriously I'd love to see how this boards looks like.

[Berni]

New versions of Altium do support multi board designs that allow you to import in multiple PcbDocs into a single file. But yeah i can see why you would want to keep it as one.

You can do it perfectly fine by simply cutting the board down the middle, inserting connectors and just drawing a board outline around both, then place a "board cutout" between them to split it up completely. The schematic will be the most work for this since net names on both sides of the connector need to be different. I typically do this by adding a ' to the end of the netname on the other side. It is easy to spot if you missed a have a duplicate net name on both sides because on the PCB you can see Altium drawing a rats nest line between the boards.

I am also curious what this board actually does since it is a HUGE board by any stretch of the imagination! Not many products even need such a massive amount of electronics (especially given how much more compact modern electronics have gotten) while devices that do need such a huge amount of electronics will typically split a design this big into about 10 boards. Not only does this make the boards much easier to manufacture, but it also makes the product easier to develop (no need to respin the whole huge expensive board for a revision) and much easier to repair (boards can be swapped around to quickly locate a fault). Id imagine such a large board in modern times would contain in the order of >10 000 components.

[free_electron]

   It is heavy and sags and bends just by picking it up.

i hope you design in busbars or stiffners or are going to support this thing properly. you will have to deal with cracked parts and fractured solder joints...
if that board cannot be kept supported during reflow it will crack parts just picking it off the conveyor... I've seen that happen.
Your other issues is going to be finding a reflow oven that has a long enough hot zone and the right speed to guarantee the correct dwell time. one part of the board will be in reflow while the other is still burning off the flux. this is going to give tremendous stress on the board.

not a good idea ...

[Alti]

it won't fit in the smt machine, won't fit into x-ray, won't fit into the reflow oven, and just plain won't fit.

What is the maximum panel size standard accepted in PCB assembly houses? Obviously this varies but there must be some kind of standard that is commonly accepted. Of course bare PCB manufacturing is one thing and then P&P process max panel size is another. I am asking for the latter.

one part of the board will be in reflow while the other is still burning off the flux. this is going to give tremendous stress on the board.

I cannot see what could be different in the process if you feed ten boards of 0.1m length one by one or just a single 1m board. I assume there are no 1m long single piece components that stretch whole length.

[mikeselectricstuff]

it won't fit in the smt machine, won't fit into x-ray, won't fit into the reflow oven, and just plain won't fit.

What is the maximum panel size standard accepted in PCB assembly houses? Obviously this varies but there must be some kind of standard that is commonly accepted. Of course bare PCB manufacturing is one thing and then P&P process max panel size is another. I am asking for the latter.

This varies for every subcontractor, depending on their equipment, and also by the type of assembly ( e.g. single/double sided, PCB thickness, stencil requirements etc.). Each part of the process will have different limits, e.g. a place I use can do up to 1.6m, but their auto stenciling system only does about 1.2m, so longer boards need to be hand-stencilled, with reduced accuracy, so it's fine for dumb LED strips, not so much with SSOP drivers on the back.
Somewhere around 350x450mm is a fairly common maximum.

[Alti]

(..)Somewhere around 350x450mm is a fairly common maximum.

I guess the machinery is made to match imperial panel sizes.
I did some investigation, some sources like this one suggests 12" x 18" (304.8mm x 457.2mm ) which is close. Also here and here. Then PCBWay have it 530mm x 330mm (close to 13" x 21").

Some sources give 18" x 24" as standard PCB assembly panel but I guess this requires really specialized gear.

Might it be that 18" x 24" size is popular for mainstream PCB production and then this is chopped in half and 12" x 18" panels slide through PCB assembly?

[free_electron]

one part of the board will be in reflow while the other is still burning off the flux. this is going to give tremendous stress on the board.

I cannot see what could be different in the process if you feed ten boards of 0.1m length one by one or just a single 1m board. I assume there are no 1m long single piece components that stretch whole length.

your 0.1m board will be hot all at the same time. that super long board will be half hot , half cold. this causes a ripple effect. i've seen boards used in MRI machines. they need special long zone ovens , or have an oven with dynamic conveyer speed.
the problem is that the total dwell time in the various zones need to be quasi constant. the flux activation time is much longer than the reflow time. so you get into issues timing the conveyor. they traditionally solve this by having a constant conveyor speed , a long flux zone and a short reflow zone. the longer you make the reflow zone the longer the flux zone needs to get. the travel speed determines the time in a zone. so if you need a hot zone of 1 meter ( which is good for a 3/5 to 3/4 meter board ) your flux zone is much longer ( 4 to 5 times that ) or you need a conveyor that can speed up ( but not too much as you don't want thermal shock ). Getting the speed and zone size right is going to be a problem. you want the board to go in fast enough , but not too fast to avoid thermal shock , sit in the flux zone for a minute or two then go through reflow for 15 to 20 seconds , then cool down.

The ovens do not ramp temperatures. this is not a converted pizza oven you use at home ! the oven is a long tunnel with various areas at different temperatures. these ovens have a large thermal mass so the zones dont influence each other and the board does not alter the inside temperature. it takes 24 to 48 hours to switch such a thing on .... altering the temperatures to accommodate 'crazy' boards will take a lot of time to reach setpoint.

your other problem will be thermal uniformity.

https://hellerindustries.com/reflow-oven/