Technique to duplicate PCB dimensions and screw hole placements?

[nuke]

I want to make an alternate board for a production amplifier. The target is mass-produced printed circuit board, I have a different circuit design I want to fit into the existing chassis and fastener placement.

Any tips for replicating 1-for-1 dimensions for the board outline and the screw holes, placement of tube sockets and so on, to create a drop-in board?

I've had varied results doing this over the years. Without the original mechanical design drawings, I usually mess something up, somewhere, somehow.

Any tricks or learned techniques to approach this work?

[R.G.]

I've done it out of necessity several times.

Steps:
0. If you don't have a CAD/mechanical drawing program, get one, and learn to use it. Make sure it can print to PDF in 1.0000000000 size.
0a. If you don't have a digital caliper, get one. Harbor Fright has these for under $20, and often under $10 for the 6" size. You'll wonder how you lived without it after a short time.
1. Measure the existing board size and mounting hole locations. Write these down, and enter the locations into the CAD design. It is a huge help if you can remove the original board and use it as a template to trace size and mounting holes. Neither of these will be perfect, so go to step 2.
2. Do your best on the CAD drawing, then print out a 1:1 version on paper, seaming and patching on multiple sheets if needed.
3. Lay the paper-dolly version in place and see how bad you did. My first one never passes this test. If it's not really close, go back to 2, making corrections the best you can.
4. If the hole locations are pretty good, all the centers actually being over holes, use that digital caliper and measure the heads and body diameters of the screws that mount it. Open up your mounting holes until they are bigger than the body diameter of the threads, but with all the opening diameter you can give them without letting the heads drop through. Make the changes on the CAD drawing.
Iterate until the paper version is pretty good, then transfer the paper layout onto 1/16" cardboard and drill holes. Try to mount that in place. When this works, you have the mounting holes and keep-out areas for putting into a PCB CAD program and finishing a layout.

Once you accept that you will make mistakes and can iterate them out at low cost by CAD-and-print, it gets pretty straightforward. And it's much FASTER than doing one version you think will be perfect - until you get the PCBs back from the fabricator and find out you missed something. Cardboard is cheap and fast.

[xtian]

I use Illustrator instead of CAD, but it's similar. If I can precicsely map out some landmarks in Illustrator, then I shoot a photo using a long lens (2X on iPhone), drop this photo into Illustrator and set opacity to 20%, then stretch the image until it matches my landmarks. This makes it easy to sketch in all required elements. Then I use digital calipers to fine tune everything.

[maxkracht]

You could also get a transfer punch set to find center a bit easier. Wouldn't need to do much actual measuring if you only wanted to make one board, just tape it down and punch on a fresh sheet of garolite. https://www.amazon.com/gp/product/B01AD ... X0DER&th=1

[nuke]

In this case, I'm contemplating something complicated enough to warrant an actual printed circuit board to retrofit into an existing chassis, including parts placement of tube sockets and jacks.

I've never been a great board layout guy, and decades of writing software hasn't improved that.

[dorrisant]

I use Corel draw to place mount holes on a blank board, the board being the exact size/shape that you need. Then you can export it and import that into Kicad where you can place and trace all of your circuit parts.

[martin manning]

...Then you can export it and import that into Kicad where you can place and trace all of your circuit parts.

Can a .pdf be imported into KiCad?

[R.G.]

I don't use KiCAD. Does it have the facility to place a pad on coordinates you type in?

I use Corel Draw for most technical drawing. FreeCAD is good for 3-D stuff, but for 2D, I'm faster with Corel. Once I get hole and other features spotted by measure -> draw -> print -> repeat to close enough tolerances, I select features on the Corel drawing, get the coordinates there, and then manually type in the coordinates of pads for mounting holes and such. This sidesteps the issue of photo distortions and pdf inaccuracies when trying to get it into the PCB program.
If, for instance, a mounting hole was at (X,Y) of (1.453, 0.625) in the Corel program, then placing pad for this hole in the PCB program and manually typing in 1.453,0.625 for the pad location in the PCB program side steps any translation errors in photo -> pdf -> pcb program.
i used this process to get true-fitting PCBs for Thomas Organ Vox preamp boards that just bolt in.

[martin manning]

I don't use KiCAD. Does it have the facility to place a pad on coordinates you type in?

Yes it does.

[nuke]

Yeah, I'm using KiCad too.

I've built some things using the print-it and fit-it iterations, which seem to work if it all fits on the laser printer.

But I admit to being not great with mechanical CAD and reverse-engineering the duplicate mechanicals fitments.

[lonote]

I have dabbled with PCBs only recently & have been using https://easyeda.com/.

From what I can tell, the preferred method is create a schematic with all your specific component part#s/footprints specified & the program will generate a physical layout, but I have never used it that way, so I am not sure about that. I skipped the schematic stage & went straight to design a PCB only.

I was designing small daughter-type boards; one for a Bandax tone circuit, one for a SS trem & another for a filtered dual bias circuit.

I was able to find generic enough footprints for my components & then manually did the component, pad & trace layout until I was happy with it. You can specify any board dimension(s), holes, etc. during that stage.

It was pretty straight forward & when you are done, the program will generate a Gerber File to have the board made.

I have started a few others with board-mounted tube sockets but haven't finished those up yet.

[R.G.]

From what I can tell, the preferred method is create a schematic with all your specific component part#s/footprints specified & the program will generate a physical layout, but I have never used it that way, so I am not sure about that. I skipped the schematic stage & went straight to design a PCB only.

That works fine for smaller boards and smaller circuits. But above a certain size, schematic entry is no longer a nit-picky time wasting process. Schematic entry tells the program which pins connect to which pins ( called a "net") and things like which pins don't connect to anything else. This tells the program what you're trying to do, and to feed back to you if you connect something that doesn't match the schematic, and also when you have forgotten to hook up pins that should have been connected. This is a huge advantage for layouts above maybe a dozen or two parts, where you maybe can't hold the entire circuit in your head.

Historically, this was the first step in automating layouts. It leaves the entire physical positioning process up to you. The next steps were to consider each of those nets to be made up of rubber band material so they could notionally pull the most-connected parts closer together. A computer could then compute the length of ALL of the nets and start arranging parts to the total length of all the nets was smallest, without any regard for the actual routing. This let the computer place the parts, re-calculate the lengths of all the nets, and tell whether a given positioning is better than another. This last is why the PCB program wants you to define footprints, so it can combine the net definitions with footprints and let the program work out positions. This let us (humans...) substitute machines' hacking for skilled humans with extraordinary brains.

I never use auto-placement or auto-routing. I have periodically tried them, and didn't like either the time spent by the computer doing the process or the results. I do the schematic entry and footprint definitions because they help me place and route more quickly and more error-free.

[martin manning]

I never use auto-placement or auto-routing. I have periodically tried them, and didn't like either the time spent by the computer doing the process or the results. I do the schematic entry and footprint definitions because they help me place and route more quickly and more error-free.

Schematic entry is essential to make sure the traces match the schematic. That doesn't mean the schematic was entered correctly, though. KiCAd can run LTSpice, which is extra insurance against that. I agree on the auto-routing. it works, but if you want to make the board conform to a specific footprint there is still work to do. It can be a leg up to get started.

[dorrisant]

...Then you can export it and import that into Kicad where you can place and trace all of your circuit parts.

Can a .pdf be imported into KiCad?

I can't recall if it will import pdf files, but I can always export whatever type of file needed for Kicad. It may be a dxf file form that Kicad will accept for this. I haven't made anything PCB in quite a while. I will check, but you can too... Just use the drop down menu and see what type of files it will allow. It is easy enough to convert a pdf to a dxf by exporting from Corel, or your app of choice.
As a note: you can import your board shape with mounts as a layer in Kicad. After you have placed all of your parts, including mount holes (which you have to include in your schematic, grounded or not), you can delete this layer for a cleaner look. I usually export this file with "crosshairs" over the centers of any holes to make placement of the hole components super easy. Then you can import another file that is just the board outline without holes. There may be a better way but this has always been easy enough and produces great results.

[R.G.]

Schematic entry is essential to make sure the traces match the schematic. That doesn't mean the schematic was entered correctly, though.

Aye, there's the rub!
There's nothing so frustrating as a machine that gives you >>> exactly <<< what you asked for, not what you meant to ask for.