Curved lines in PCB design - Page 1
Forum section: electronics / beginners

author: Liffraun-N
author_rank: Newbie
timestamp: June 15, 2025, 02:26:01 pm
content: Hello, I would like to digitize and then manufacture such an old board, but I encountered a problem when choosing a program that could help me with this.The thing is that this board (and three more auxiliary boards of this device) have non-standard curved pads for contacts.Basically, I need to outline these pads with curved lines, and then make these curved perimeters solid (fill).In tutorials on popular programs, I did not see anything similar to what I need. Because, in modern times, it is customary to distribute everything with ordinary angular buses.But maybe there are other ways?It's just... Unfortunately, I do not have enough experience in electronics to try to remake this (and other) boards in a modern way.After all, these boards were designed by smart people, for a considerable current of a large number of transistors.I would like to repeat exactly, for starters.

author: Vovk_Z
author_rank: Super Contributor
timestamp: June 15, 2025, 02:57:30 pm
content: Usually there is no need to replicate it as is. You may use any wires, except some where really large currents are present

author: PGPG
author_rank: Frequent Contributor
timestamp: June 15, 2025, 03:20:15 pm
content: I didn't explored it too much, but in KiCad when you enter and exit pad edition than all copper connected with that pad becomes a part of that pad.

author: tooki
author_rank: Super Contributor
timestamp: June 15, 2025, 03:44:41 pm
content: While I agree that there is no technical reason to reproduce the exact shapes from the original board, the key concept in doing so is that you won’t use tracks (lines) at all, but polygons. I know for a fact that Altium can do what you want. I assume KiCad can too, but I couldn’t tell you how.

author: KrudyZ
author_rank: Frequent Contributor
timestamp: June 15, 2025, 03:58:01 pm
content: This will be tedious, but the quickest way might be to use trace paper to just get the outlines of the copper and then scan it in.Convert the image to a vector format and export as DXF which you can pull into a PCB program an convert to polygons.There might be some more direct way for the latter steps, but I think that removing the extraneous information in the print you have will be where automated ways will struggle, therefore my proposal to manually trace it.

author: Zoli
author_rank: Frequent Contributor
timestamp: June 15, 2025, 04:00:14 pm
content: To do it with KiCad, you will need Ver9.x.x; it allows you to use curved lines(Bezier curves). Use the tool to draw the outlines of the pads, then draw an approximate outline to fill that pad; now all you have to do to place the the parts.I've attached a short demo of what I've written above.

author: Simmed
author_rank: Frequent Contributor
timestamp: June 15, 2025, 04:09:46 pm
content: hmmm i have imported graphics into eagle beforeso i know for sureyou could clean up the jpg and (scale it properly) then convert it to bmp (8bit)then eagle could import it as a bmp layerthen inside eagle (already to scale)just draw the tracks by hand and "write" the component mask manuallyyou can also draw polygons, bend the polygons, make it curve, etcthere is also the chance to add additional "component" footprints for modern equivalent or even shift things aroundit will take some clever assignment of hotkeys to display layers (ie show diagram, hide diagram, etc)i think it will take about 2 days maybe

author: mariush
author_rank: Super Contributor
timestamp: June 15, 2025, 04:11:11 pm
content: Another option would be something in-between ... rearrange the components so that you'll have squares, rectangles, L & T shapes made out of copperIt would speed up creating the copper fills using basic shapes instead of curvesAlso consider tweaking where possible to use surface mount resistors instead of through hole parts. 1206 resistors can nicely sit across two such fill regions.

author: wraper
author_rank: Unknown
timestamp: June 15, 2025, 04:16:42 pm
content: It's also an quite ugly and suboptimal design where all jumper wires can be replaced with traces even without rearranging any parts and not adding any copper layers. Also no mounting holes whatsoever. I would not bother to replicate ugliness for it to be an exact match. Also it apparently uses axial capacitors, which is another reason to not replicate it exactly.

author: eugene
author_rank: Frequent Contributor
timestamp: June 15, 2025, 04:22:51 pm
content: The usual workflow is to create a schematic, assign footprints to all of the components, "Update PCB" from schematic, arrange the footprints, then use the rats nest to layout traces. This is an absolutely essential process for any new designs.Having said that, this is not a new design. What I would probably try is to create a graphics image of the copper layer. Import the image into a user layer in the KiCad PCB editor, then change the layer to front copper. From there you'll need to add through holes (vias) where appropriate. If you want solder mask then you'll need to set up the vias to have large annular rings that don't get solder mask.If all that you have to start with is the image in your post, then a few hours with a graphics program can clean it up by removing the components, jumper wires, etc.If you happen to have the original PCB with all the components removed then you can scan it to a pdf file. KiCad might import pdf directly. If not, use Inkscape to covert to a different format.

author: pcprogrammer
author_rank: Super Contributor
timestamp: June 15, 2025, 04:26:47 pm
content: Another option is to draw out the schematic in a modern tool and use that to design a new and modern PCB for it. After drawing the schematic things like current drawn will become clear and suitable trace widths can be chosen to make the PCB.Component can be replaced with modern SMD types and placement can be optimized. The result may even be better than it was in the old days.Unless sentiment and retaining original-ness is needed or wished for, there is no need to stick to the old.eugene typed faster than me.

author: Liffraun-N
author_rank: Newbie
timestamp: June 15, 2025, 05:04:04 pm
content: Thank you very much, guys. Your answers were very informative. Got it all!

author: Doctorandus_P
author_rank: Super Contributor
timestamp: June 16, 2025, 10:47:04 am
content: I'm not sure whether it's clear from the previous posts, but there is nothing special about this PCB. The reason it looks like that is because it is a very old design, probably made back in the '70-ies. Such PCB's were hand drawn. This predates the '80-ies where home computers firstly became available.So you have a bunch of options.If you want to preserve the aesthetics, you can scan the PCB, import it in a PCB design program on a copper layer and then just add holes (footprints with a single THT hole) or place footprints for resistors and capacitors and such on top of the graphics. You can also opt to import the graphics on an "auxiliary" / User layer as an aid to draw tracks, or completely reverse-engineer it.

author: Infraviolet
author_rank: Super Contributor
timestamp: June 17, 2025, 07:09:32 pm
content: Just to make the point that hasn't been made yet, but which the OP might be interested in...In practice there's certainly nothing "wrong" with curved traces on PCBs, it might not be the "done thing" today, because most design software defaults to using horizontal, vertical and 45 degree angles, but there's no electrical or manufacturing reason against doing so (most of the time, ignoring things like really fast RF stuff). The "no acute angles" rule was, it doesn't matter much now with more recent developments in PCB manufacturing production lines, always about etchant acid getting trapped in tight corners and eating away at traces, thinning or breaking them, it was never an electrical matter. Except for really fast RF stuff, curved designs are just as trouble-free as tight angles. Curves on an old board design mean it was quite probably designed by marking out which pins were on the same "net" as others, then literally drawing on lines for where the copper plating should be etched away so as to separate the different nets.

author: xvr
author_rank: Frequent Contributor
timestamp: June 18, 2025, 01:05:50 pm
content: QuoteJust curious, there is at least one autorouter that uses curved traces -https://en.wikipedia.org/wiki/TopoRExample:

author: MarkF
author_rank: Super Contributor
timestamp: June 18, 2025, 01:39:33 pm
content: I don't know if KiCad can do it or not.Diptrace can import a black-and-white photo into the silk screen layer. For example, placing a logo on the PCB. Diptrace will also allow you to place the image on the signal layer which ends up like a copper pour. You would need to do some photo manipulation and scaling and place individual pads for the component holes. But for your PCB, precise placement and scaling won't effect through-hole parts. For a 'one-of' replacement of an old PCB that was probable drawn by hand, it would be do-able.

author: MarkF
author_rank: Super Contributor
timestamp: June 18, 2025, 02:35:22 pm
content: Here's a crude example of the results of the upper left corner of your PCB.You would take more care when doing the drawing and you could do asecond drawing for the silk screen.