Hi all, absolute newbie first-day guy here, sorry in advance. So, I’ve got a pretty frustrating situation here with a simple little single-sided FR4 PC board that dates from the early 90s, that I need to get some more made of. The company in Boulder CO who made them for me over the…decades, went out of business on me. All I’ve got for the little guy is a ‘filmwork’ 1:1 negative plastic film thing (the traces and pads are transparent, on a black background), and an actual ‘sample’ board…no Gerber files. I’m thinking KiCad can probably help me here, but boy am I clueless. Does anyone here know of a straight-on tutorial for this specific issue? Any thoughts would be really appreciated. C. Hale, Boulder CO
Well, you can either redraw it in KiCAD or some other program, or you can look for a company still running antique PCB processing.
I’m not aware of any “film-to-Gerber” software.
Thanks for your thoughts here. I did find something, maybe, Image to PCB – Create all files to manufacture a PCB from an image (wordpress.com) “Image to PCB”. It sounds like what I want to do, but, I’m frankly not sure. --Charley
It being a “simple little single-sided” board, I would think it is worth considering the option of redrawing it in KiCad, especially if the circuit diagram is already known.
The process would be essentially identical to the reverse-engineering of an existing board, only you scan the films and insert the scanned picture of them into the board editor for reference, instead of a photo of the existing board.
The process has been described fairly recently, even I wrote a quick outline of it recently on this forum.
I have done a couple, and it is not that bad after all. And then you can easily make new revisions too, if you want or need to.
1 Like
Were you able to find a solution to your problem yet?
Reconstructing an old design from a few old files and pictures can be a frustrating and time-consuming project, sometimes with less than stellar results. There’s several threads here that discuss the issues when trying to recreate an old design. I’d suggest that before you worry about recreating the PCB you should see if the parts are still available. There’s been lots of churn of parts vendors (i think you’re talking about 30 years old, no?). it might be easier and cheaper to redesign it with new parts and use the outline of the old board to make it fit your application. The best part of re-doing the design in KiCad would be that you’d never lose access to the original design files again!
2 Likes
I think this is solid advice
I think one of the biggest potential issues with a “stupid copy” is getting through hole pin spacing correct, if you can find all the original components.
but
If you want to keep the design for another 30 years you may need to update the files to a new version of Kicad every few years. (??)
I also encourage you to go to SMT if that is appropriate. I and many others on this forum could provide some guidance on that if you want it. SMT may have a few advantages, possibly including saving a bit of money on components unless you have all of them already.
Is it possible to scan the negative, and import it to copper layer?
That would be a graphic and you cannot connect nets to it or use DRC. Holes would have to be guessed.
PCB fabs won’t like it as they cannot do an electrical check.
Scanning the plot and importing to a technical layer, redrawing the schematic and placing footprints to align is a much better way to get an accurate design, that can easily be amended if parts have to change.
You could scan the negative, vectorize it (for example with inkscape) and then import it as polygons on a copper layer. However that would not give a clean result, editing it will be cumbersome and DRC will have lots of complaints and you couldn’t check clearances or manufacturability properly. And as @davidsrsb wrote, via/hole locations might be a problem.
But it’s an option if you just need something quick an dirty. Reverse engineering it is definitely the proper solution.
Non-sequitur but I sometimes yearn for the curvy copper patterns of yore. Geometrical tracks are so boring if functional.
1 Like
FWIW, I like Latin and elevated language 
1 Like
The Round Tracks plugin makes curvy tracks. Useful to clone old hand drawn boards
Yeah but I want curvy areas too, like those old PCBs from the far east where the copper layer (one!) is covered by blobs. Elektor designs were like that too.
Hi all, thanks very much for all your replies to my predicament here, I’m still absorbing. Meanwhile, I completely ‘redrew’ the thing in AutoCAD (2017) using polylines throughout, so this ‘model’ is totally solid and ready to do…something with, seems to me. But what, exactly?? I was just poking around looking at Autodesk Eagle (…which I guess expired at the company on 6-7-23…but it did download ok it appears to me, associated with a separate subscription I have for Fusion 360). Is there a straightforward way for me to take this ACAD .dwg file of the board pads/traces, and get where I need to get in terms of Gerber files and ‘drill file’? (I know precisely what the three different drilled hole diameters are, no problem there–) Thanks again for helping this newbie…—Charley
–by the way, I’m also really poorly educated as to the use of Fusion360 Design, too; the only reason I have it is for its CAM functionality. I have SolidWorks and I import my SW models into F360 CAM to generate toolpaths and post files for a CNC mill I have. So anyhow, I’m woefully unlearned in F360 Design, too…–
First, the Best approach is to completely re-draw the PCB in Kicad.
Second, if having already done everything graphic/3D-model, export as DXF and use it in Kicad.
Third, Using the Negative, as follows:
Using a Negative… The Steps
- Take a Photograph of the Negative with White Paper underneath it. Save it to computer as either: PNG, JPG, TIFF (prefer PNG)
You need to know it’s Scale so, do this:
• You need to know at least One dimension on the Negative’s image of something on the PCB.
Example: Let’s say you know there’s a Chip on the PCB/negative and know it’s Pitch-Spacing between PAD’s is O.1inch (2.54mm).
• Grab some Calipers/other and measure the distance between two adjacent Pad’s on the Photograph. Say it measures 4.5mm (0.177 inch).
Thus, Scale-Factor = 0.1/0.177 = 0.565 inch (= 2.54/4.5 = 0.56 mm)
-
In Kicad’s main panel, Select the “Image Converter” tool and load the PNG/image (the button says ‘Load Bitmap’).
Select the Tab ‘Black&White Picture’ to get best resolution and use the Threshold Slider to adjust for the best/cleanest image. -
Set the Size boxes to appropriate units and set the ‘Lock Ratio’ to Locked by clicking it if needed. Enter the Values for the two boxes by calculating the two shown values by the Scale-Factor.
Example: if Box shows 182.5mm, then calculate 182.5 X 0.56 = 101.2. Do similar Calc for the other Box if not wanting to maintain Aspect Ratio.
-
Select ‘Output Format’ for Footprint and set ‘Board-Layer for Outline’ to User layer Eco1. Check or UnCheck the Negative Box, as you desire.
-
In Kicad’s PCB editor, load the newly saved Footprint
-
Now, you have some Usage Options:
• To Move Items to desired Copper Layers: Double-Click items to change to desired Layer
• To use for Placing Items/Footprints/etc and drawing Traces, use the Footprint as-is but, might prefer to Invert from Negative when in Step#4, above.
• Naturally, if your image contains the PCB-Shape, change the shape lines to Edge_Cut layer
Screenshots show the above and a Placed Resistor (I did NOT accurately do the Scaling for this example - just assumed geometry to dempnstrate the Process Steps…)
1 Like
Blackcoffee, wow, thanks very much for providing this. I’ll try to absorb it and make use of it. A bit ago I sent my .DXF file of the ‘polylines-only’ scale drawing of the board/‘mask’, and a quick ‘spec sheet’ with the three necessary through-hole diameters for the board and etc., to folks in India who I found good feedback about on the web, Rapid Circuit. I hope they can take these materials and turn around a dozen of the little board, and I’ll be done for now. But I’m definitely going to review what you provided here, too. Thanks again to you and everyone who’s weighed in on this, which I can well imagine you’ve all been over many times in the past…–Charley
1 Like
As a follow-up:
There are a number of ways to accomplish your goal and much will depend on the info/files you have at hand and/or are willing to create.
As a separate example, since you say you have ‘DXF’, you can simply Import the DXF into Kicad, then Plot the Gerbers. Assuming you know what to do with the Gerbers…
I CNC Mill my PCB’s and use CopperCAM to get the Gcode for milling (the limited, Free use is useful for small projects/testing).
Here’s a quick video of Using a DXF in Kicad and Plotting the Gerbers. Then, I quickly loaded Gerber into CopperCAM but I did NOT fuss with detail-work (or select desired Mill Bits or the Drill…etc) in either Kicad or CopperCAM for this Video demo - it’s enough to convey the concept/ideas though…
And, I want to emphasize, it will be Quicker, more useful and will provide future ability for changes…etc if you Start A New PCB in Kicad and do all the PCB work. You will learn Kicad and end-up with something useful…
I don’t use FreeCAD’s Path workbench for PCB milling but, I do use it for general Milling.
For fun, I put together this YouTube video on using FreeCAD for Milling PCB…