EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => Topic started by: MaximRecoil on November 24, 2016, 04:05:11 pm
-
For example, if I wanted to recreate an existing PCB, the easiest way to do it would be to scan the PCB in at e.g., 600 DPI, drag the image into design software, set the opacity to about 50%, and then layout the PCB design on top of it, using it as a guide. When finished, the image can be deleted. That's exactly how I would do it in e.g., Adobe Illustrator, but unfortunately, vector files aren't used for manufacturing PCBs (not that I know of anyway). There's no technical reason why they couldn't be used, provided a standard method of layering was agreed upon, i.e., put the silkscreen layout on one layer, the drill holes on another layer, and so on.
In any case, is there any PCB design software that allows for that? It would save me from having to do a bunch of manual measurements to determine trace/pad size, positioning, and shape.
-
Some PCB packages will import vector-based formats like DXF and/or gerber, so if you can get to one of those you may stand a better chance.
-
I have Cadsoft Eagle. Can it do that? If not, which ones can?
-
Circad will do this for you, but it would be unusual to buy a CAD package for this type of one-off requirement.
http://holophase.com/features.htm (http://holophase.com/features.htm)
Half way down the above webpage "A Tool for Reverse Engineering"
-
Circad will do this for you, but it would be unusual to buy a CAD package for this type of one-off requirement.
http://holophase.com/features.htm (http://holophase.com/features.htm)
Half way down the above webpage "A Tool for Reverse Engineering"
That's awesome. It reads almost exactly like my original post, including the part about deleting the image when you're done:
With pixel images integrated into PCB data files, reverse engineering a circuit becomes as simple as placing actual parts and tracks on top of the pictures of the parts and the tracks. An assortment of pixel image processing functions are available to rotate, scale, and transform the images so they are properly grid-aligned with the real world. Once the new layout is complete, the superfluous image data can be discarded.
Why doesn't all PCB design software have such functionality?
-
Eagle can already import bitmap images, can't it? It will divide them into layers based on colour and display them as rectangle blocks. But with properly cleaned-up images that should do the job well enough, shouldn't it?
-
This is quite a coincidence. I've been emailing back and forth with someone who has done quite a few nice reproductions of ancient PCBs, and I asked him what he uses for PCB design software. I didn't mention anything about wanting to use an image as a guide, but this is what he said:
For the reproductions I am using Sprint Layout
(http://www.abacom-online.de/uk/html/sprint-layout.html (http://www.abacom-online.de/uk/html/sprint-layout.html)),
you can load a JPEG image as a background for the PCB design.
Using this way you can re-draw the board. For my own designs
I am using Eagle.
Given his excellent results, I think I'll give that a try.
-
I have Cadsoft Eagle. Can it do that? If not, which ones can?
DipTrace can import DXF and Gerber files. If you have a PDF file that contains a layout, you can use "pstoedit" to convert it from PostScript to DXF.
For raster images, DipTrace will also allow you to apply a BMP/PNG/JPEG as a Silk/Assembly/Paste/Copper layer. So long as you crop and scale your image in a vector editor (GIMP/PhotoShop/Pixelmator) it should work fine. (Be aware the import will flatten the image to black and white (not grayscale), so you might want to do that yourself in a image editor before hand.)
Edit: Once I scanned an old PCB and separated the traces from pads into separate layers using my photo editor, then I ran the layers through an online raster to vector converter, took the resulting SVGs and converted them to a single multilayer DXF and imported it into DipTrace. During import, DipTrace let's you assign each DXF layer to something different (pads, top and bottom copper, silk, paste, etc.), which allowed me to have a fully editable version of the board that I could produce Gerbers from.
-
Edit: Once I scanned an old PCB and separated the traces from pads into separate layers using my photo editor, then I ran the layers through an online raster to vector converter, took the resulting SVGs and converted them to a single multilayer DXF and imported it into DipTrace. During import, DipTrace let's you assign each DXF layer to something different (pads, top and bottom copper, silk, paste, etc.), which allowed me to have a fully editable version of the board that I could produce Gerbers from.
That sounds like a nice way of doing it. Personally, I would vectorize the raster image manually, because that sort of thing is my specialty (I'm a screen printer; everything I print is from vector files). That's a good option for me to consider. Thanks.
-
In answer to your earlier question whether Eagle can import DXF, the answer is yes. In my version, it is a ulp. I don't know about the lastest version. The program I use is "import-dxf-1_6.ulp." I use it quite frequently when needing a complex geometry. You can important into almost any layer. I generally use the dimension layer. Oh, and be sure to specify in the import dialog whether the dimensions are imperial or metric.
John
-
Edit: Once I scanned an old PCB and separated the traces from pads into separate layers using my photo editor, then I ran the layers through an online raster to vector converter, took the resulting SVGs and converted them to a single multilayer DXF and imported it into DipTrace. During import, DipTrace let's you assign each DXF layer to something different (pads, top and bottom copper, silk, paste, etc.), which allowed me to have a fully editable version of the board that I could produce Gerbers from.
That sounds like a nice way of doing it. Personally, I would vectorize the raster image manually, because that sort of thing is my specialty (I'm a screen printer; everything I print is from vector files). That's a good option for me to consider. Thanks.
Yes, at the time I only had Pixelmator (which is like a nice lightweight alternative to Photoshop on macOS) and it was quicker for me to do it like that. These days I'd use AutoDesk Graphic (formerly iDraw) and import the scanned board as a raster layer, then trace over it with vector paths. I'd then export it as a PDF and run it through "pstoedit" which is a great little CLI program that converts PostScript files to tons of different vector formats, including DXF.
I've used the Graphic -> PDF -> pstoedit -> DXF workflow a lot lately to create custom, intricate pad shapes for DipTrace and it works surprisingly well. Dimensions are maintained perfectly throughout the conversion process.
-
This Adafruit tutorial on Creating Accurate Footprints in Eagle (https://learn.adafruit.com/creating-accurate-footprints-in-eagle/overview) uses a technique of importing a bitmap file for a footprint outline, which the designer then traces and later deletes. This same technique could probably be used for your entire PCB duplication.
-
I've used the Graphic -> PDF -> pstoedit -> DXF workflow a lot lately to create custom, intricate pad shapes for DipTrace and it works surprisingly well. Dimensions are maintained perfectly throughout the conversion process.
I really like this idea, because I can very accurately reproduce almost anything in Illustrator; the drawing tools are far superior to anything you'd find integrated into a PCB design program; drawing is Illustrator's specialty, and it's the de facto industry standard. This would be especially good for the silkscreen layer, because in Illustrator I can match text exactly, even if I don't have the correct font. Plus, I've been using Illustrator for about 12 years, so that alone makes things a lot easier.
Illustrator can export to .DXF, though there are sometimes issues with its .DXF files when used in AutoCAD. As long as they stay 2D they are fine, but I've seen some weird anomalies when extruding them to 3D. I had a trial program whose sole function was to convert .AI and .PDF files to .DWG and .DXF, and that did a beautiful job ("pdf2cad"), no issues even when extruding to 3D. It sounds like pstoedit may be just as good, and it's free. I see it uses ghostscript, which I've used in the past (along with GSView) for effectively turning my printer into a Postscript printer (which allows me to print halftone film positives for screen printing; you'd normally need a Postscript printer or [expensive] RIP software (such as Accurip) to do that.
-
I've used the Graphic -> PDF -> pstoedit -> DXF workflow a lot lately to create custom, intricate pad shapes for DipTrace and it works surprisingly well. Dimensions are maintained perfectly throughout the conversion process.
I really like this idea, because I can very accurately reproduce almost anything in Illustrator; the drawing tools are far superior to anything you'd find integrated into a PCB design program; drawing is Illustrator's specialty, and it's the de facto industry standard. This would be especially good for the silkscreen layer, because in Illustrator I can match text exactly, even if I don't have the correct font. Plus, I've been using Illustrator for about 12 years, so that alone makes things a lot easier.
Illustrator can export to .DXF, though there are sometimes issues with its .DXF files when used in AutoCAD. As long as they stay 2D they are fine, but I've seen some weird anomalies when extruding them to 3D. I had a trial program whose sole function was to convert .AI and .PDF files to .DWG and .DXF, and that did a beautiful job ("pdf2cad"), no issues even when extruding to 3D. It sounds like pstoedit may be just as good, and it's free. I see it uses ghostscript, which I've used in the past (along with GSView) for effectively turning my printer into a Postscript printer (which allows me to print halftone film positives for screen printing; you'd normally need a Postscript printer or [expensive] RIP software (such as Accurip) to do that.
Exactly! Since you've got Illustrator, you should be able to churn out pretty much anything you'd need vector wise.
One nice thing about pstoedit is it gives you fine grain control over the conversion. For instance, you can convert to two different types of dxf files: Plain DXF and DXF_S (which supports splines). You can also add switches that can convert splines to polys or even polys to lines, and you can do it with whatever precision you desire (which controls how many points it produces when turning a spline to a poly or a series of lines).
Now, that may not be important in Eagle, it might support DXF files with splines, I'm not sure; DipTrace doesn't, so it's very nice to be able to convert them to polys.
I use it under macOS, but it should work under Windows just fine if you've got Ghostscript. I love GS as well! I've got it setup in my Windows 7 VM to provide a virtual PDF printer. It's so handy to be able to "print" a schematic directly to a PDF.
My current project involves a cap touch panel with a large number of buttons; using GS I can "print" my board layout to a PDF and then import that into my vector editor, AutoDesk Graphic. Now I've got an exact copy of my board outline with the exact position of the buttons (that's fully editable since it's vector) which I can use to create the silkscreen markings and laser cutting pattern for the acrylic overlay that goes on top of the cap touch PCB! That saves me a ton of time that I'd otherwise spend recreating the board in Graphic.
Let me know if you need any help with pstoedit, it has a lot of options so it may seem daunting at first, but I've found it's actually pretty easy to use once you narrow down the options. :)
Edit: Oh, something else I've found handy lately, is when I'm creating a new part in my PCB software, I start by importing a manufacturer's assembly drawing PDF into Graphic, cleaning it up so only the drawing of the component remains (deleting the dimensions, arrows, etc.), scaling it and then converting it to a DXF file. I then import that to the assembly layer of the part I'm creating in DipTrace. Saves me a *ton* of time drawing the assembly by hand.
I've done this about a dozen times in the last week while looking for the right LCD for this project. It allows me to see exactly how it will fit on my board.
-
Have a look at http://www.abacom-online.de/uk/html/sprint-layout.html (http://www.abacom-online.de/uk/html/sprint-layout.html)
-
Let me know if you need any help with pstoedit, it has a lot of options so it may seem daunting at first, but I've found it's actually pretty easy to use once you narrow down the options. :)
As a test, I drew some random traces in Illustrator, saved as a PDF, then converted to DXF in pstoedit. I opened DipTrace > PCB Layout, then File > Import > DXF. It brought up this screen - http://i.imgur.com/PexYIjC.png (http://i.imgur.com/PexYIjC.png).
In the drop-down menu for "Convert to:", which do I select in order for that to become the top traces? Also, can I draw the pads as part of the traces in Illustrator, like this - http://i.imgur.com/13tTMCG.png (http://i.imgur.com/13tTMCG.png)? Or would I have to import the pads as a separate DXF file?
-
Let me know if you need any help with pstoedit, it has a lot of options so it may seem daunting at first, but I've found it's actually pretty easy to use once you narrow down the options. :)
As a test, I drew some random traces in Illustrator, saved as a PDF, then converted to DXF in pstoedit. I opened DipTrace > PCB Layout, then File > Import > DXF. It brought up this screen - http://i.imgur.com/PexYIjC.png (http://i.imgur.com/PexYIjC.png).
In the drop-down menu for "Convert to:", which do I select in order for that to become the top traces? Also, can I draw the pads as part of the traces in Illustrator, like this - http://i.imgur.com/13tTMCG.png (http://i.imgur.com/13tTMCG.png)? Or would I have to import the pads as a separate DXF file?
I don't think pstoedit can do multilayer DXF files, so what I'd do is export each layer from Illustrator as a separate PDF, convert each to DXF and import each as a separate object. Make sure up at the top right hand side of the import window you change it from "New" to "Add" so it imports each DXF onto your existing design.
For top side traces (well, copper in general) you'd select "Top" from that list, which is the default name of the top copper layer.
For through hole pads, the second image you posted will work, however I'd move the "inner circle" (the actual hole itself) of each pad to a separate layer, then import them separately as holes.
*Or* you could have three layers: Traces, pads, holes. That way, when you import the "pads" layer it can be applied to both sides of the board.
So, the first import would be the copper traces. The second would be copper pads (which would essentially show up as completely filled circles). The last layer would be the drill hits. That's also how a Gerber file is interpreted. (A drill hit centered on a copper pad is considered a plated through hole.)
Alternatively, you could only draw and import the traces (like your first image) and then use DipTrace to drop your SMD/PTH pads and holes. It's pretty simple to do, just click the "pads" button, drop them where you want, double click and select if they should be through-hole or SMD.
Also, when you do the pstoedit conversion, you might want to specify "dxf: -mm" and then set the Units option in the import window in DipTrace to Millimeters. That way you can make sure the scale is kept.
Oh, one more thing, be sure to define your board outline as well: Object -> Board Points. :)
-
For through hole pads, the second image you posted will work, however I'd move the "inner circle" (the actual hole itself) of each pad to a separate layer, then import them separately as holes.
I was wondering about doing it that way, and you answered it before I asked. I have designed, and had manufactured, one very simple PCB, about 4 years ago. I did it in Eagle, but all I did was follow a multipart tutorial on YouTube and substitute my design for the one in the tutorial. I didn't retain much of it. I remember the multiple output files deal is rather convoluted (.cmp, .drd, .plc, .pls, .sol, and so on) compared to files I'm used to dealing with (such as vector files), where you can put all your layers in one file and call it good. It strikes me as some sort of legacy system that is so well ensconced in the industry that no one wants to change it.
*Or* you could have three layers: Traces, pads, holes. That way, when you import the "pads" layer it can be applied to both sides of the board.
So, the first import would be the copper traces. The second would be copper pads (which would essentially show up as completely filled circles). The last layer would be the drill hits. That's also how a Gerber file is interpreted. (A drill hit centered on a copper pad is considered a plated through hole.)
Alternatively, you could only draw and import the traces (like your first image) and then use DipTrace to drop your SMD/PTH pads and holes. It's pretty simple to do, just click the "pads" button, drop them where you want, double click and select if they should be through-hole or SMD.
Also, when you do the pstoedit conversion, you might want to specify "dxf: -mm" and then set the Units option in the import window in DipTrace to Millimeters. That way you can make sure the scale is kept.
Oh, one more thing, be sure to define your board outline as well: Object -> Board Points. :)
Awesome information; thanks. I'll most likely have more questions once I get started. Before I can get started I have to depopulate the PCB that I intend to reproduce and scan it in, and before I do that, I'm waiting for some sockets and other parts in the mail. I figure I might as well put in some new parts if I'm removing everything anyway. Fortunately, it is a small PCB (74 x 74mm) and doesn't have many parts (7 DIP chips and some resistors and capacitors, all through-hole).
-
For through hole pads, the second image you posted will work, however I'd move the "inner circle" (the actual hole itself) of each pad to a separate layer, then import them separately as holes.
I was wondering about doing it that way, and you answered it before I asked. I have designed, and had manufactured, one very simple PCB, about 4 years ago. I did it in Eagle, but all I did was follow a multipart tutorial on YouTube and substitute my design for the one in the tutorial. I didn't retain much of it. I remember the multiple output files deal is rather convoluted (.cmp, .drd, .plc, .pls, .sol, and so on) compared to files I'm used to dealing with (such as vector files), where you can put all your layers in one file and call it good. It strikes me as some sort of legacy system that is so well ensconced in the industry that no one wants to change it.
Yes, what you exported from Eagle to have the PCBs made are called Gerber files. It's a vector format designed specifically for PCB manufacturing use that's at least 30 years old now.
Each of those files represents a different layer: Top Silk, Bottom Silk, Top Copper, Bottom Copper, Top Mask, Bottom Mask, Top Solder Paste, Bottom Solder Paste, the Board Outline and so forth.
Holes are exported in a format called NC Drill. This file lists the various sizes of drill bit needed and tells the drill how to move and when the bit should go up or down. It's not unlike the HPGL format used for plotters.
The reason these "layers" are in separate files is because, traditionally, each step of the PCB creation involved different pieces of equipment and completely separate masks. Even today, producing a PCB requires a lot of "hands on" and is still labor intensive. Yes, there is automation for each step, but someone still has to move the racks of panels between processes and oversee everything.
I was thinking about these files you're exporting from Illustrator... Right now, you're exporting each layer as a separate PDF and running them through pstoedit, right? Well, if Illustrator supports native DXF exporting, you might be able to save some time and see if you can export a *single* multilayer DXF file. DipTrace *does* support those.
Awesome information; thanks. I'll most likely have more questions once I get started. Before I can get started I have to depopulate the PCB that I intend to reproduce and scan it in, and before I do that, I'm waiting for some sockets and other parts in the mail. I figure I might as well put in some new parts if I'm removing everything anyway. Fortunately, it is a small PCB (74 x 74mm) and doesn't have many parts (7 DIP chips and some resistors and capacitors, all through-hole).
Great! I think this system will work alright for you. I'm here to help. :)
-
... That's exactly how I would do it in e.g., Adobe Illustrator, but unfortunately, vector files aren't used for manufacturing PCBs (not that I know of anyway).
Err, actually PCBs are created using vector files, the common format uses is Gerber Photoplot file variants, and Excellon Drill file variants.
... Also, can I draw the pads as part of the traces in Illustrator, like this -
Whilst you could do that, for some special cases* of output, you probably are better using round entities for PADS and Holes.
*One special case for that outline-mode, could be if you wanted to use a Milling machine to cut bare copper for your PCB.
If you want to use more conventional PCB FAB of silk-screened PCB and plated thru solder masked holes, then see below.
... drawing is Illustrator's specialty, and it's the de facto industry standard. This would be especially good for the silkscreen layer, because in Illustrator I can match text exactly, even if I don't have the correct font. Plus, I've been using Illustrator for about 12 years, so that alone makes things a lot easier.
If you are an Illustrator Guru, and do not want overly complex PCBs as in " Fortunately, it is a small PCB (74 x 74mm) and doesn't have many parts (7 DIP chips and some resistors and capacitors, all through-hole)."
a quick Google finds others have been before you ... look at this - PDF to Gerber is exactly what you want, as it also does the Holes, and manages solder mask and silkscreen...
http://swannman.github.io/pdf2gerb/ (http://swannman.github.io/pdf2gerb/)
pdf2gerb: Convert PDF to Gerber and NC Drill formats
The author even says this - exactly the Adobe Illustrator flow you are after!! :)
"I prefer to design circuit board layouts in Adobe Illustrator — it's a familiar tool and I get results quickly. PCB manufacturers expect designs in Gerber + NC Drill format, however, and the best Illustrator can do is export to PDF."
That's all you need. No additional CAD to learn, and no redrawing / tracing ....
-
I tried pdf2gerb when I was trying to replicate the board I was discussing earlier and had very poor results with it. That's why I ended up going the PDF -> DXF -> DipTrace route.
It might work for a one off, so the OP should give it a try, but I wouldn't expect too much out of it.
-
For through hole pads, the second image you posted will work, however I'd move the "inner circle" (the actual hole itself) of each pad to a separate layer, then import them separately as holes.
I imported the holes file but they didn't show up. I imported the board outline first, then the traces, then the pads, and those all showed up fine. I tried all of the relevant import options, i.e., importing them as "pad holes", then trying it as "all holes", then "Mt Holes", and none of them worked. I was able to click on pads, set them to through-hole, specify a hole size, and that worked.
If all else fails I could do all the pad holes like that, then import my holes file as anything other than one of the holes options (such as a silkscreen layer) so that it shows up, then use the "place mounting hole" function to place the non-pad holes, using my holes file as a guide.
Is there any way to get more precision from the pstoedit PDF-to-DXF conversion? Everything is showing up in DipTrace as crude polygons instead of circles/curves:
(http://i.imgur.com/Rvd9yuD.png)
When creating the bottom silkscreen file, are you supposed to mirror it?
I was thinking about these files you're exporting from Illustrator... Right now, you're exporting each layer as a separate PDF and running them through pstoedit, right? Well, if Illustrator supports native DXF exporting, you might be able to save some time and see if you can export a *single* multilayer DXF file. DipTrace *does* support those.
I tried an Illustrator-export-to-DXF before trying pstoedit, and it just showed up as semi-random garbage when DipTrace tried to import it.
-
I tried pdf2gerb when I was trying to replicate the board I was discussing earlier and had very poor results with it. That's why I ended up going the PDF -> DXF -> DipTrace route.
It might work for a one off, so the OP should give it a try, but I wouldn't expect too much out of it.
I've not tried it myself, but scripts like that will always be quite tool-specific - ie not work with any PDF, but should work ok with Illustrator-generated PDF, and only with the settings they give.
Which versions of Illustrator, and pdf2gerb, did you try ?
-
When creating the bottom silkscreen file, are you supposed to mirror it?
Usually bottom copper text and silkscreen text are mirrored in the PCB CAD so you get a sensible viewing system.
Some PCB tools allow a flip to bottom view, which changes the viewpoint.
At plot time, it is optional if you mirror-back the bottom silkscreen etc, as the PCB FAB will also sort that.
It is a good idea to have some label text on all plot layers, so the PCB FAB can easily see 'which way round' it needs to be.
-
I tried pdf2gerb when I was trying to replicate the board I was discussing earlier and had very poor results with it. That's why I ended up going the PDF -> DXF -> DipTrace route.
It might work for a one off, so the OP should give it a try, but I wouldn't expect too much out of it.
I've not tried it myself, but scripts like that will always be quite tool-specific - ie not work with any PDF, but should work ok with Illustrator-generated PDF, and only with the settings they give.
Which versions of Illustrator, and pdf2gerb, did you try ?
I tried it (Illustrator CS4 and pdf2gerb 1.6, which seems to be the latest version), and the output files were garbage.
Apparently the DXF format doesn't support bezier curves, which is bizarre. One of the PCBs I want to duplicate appears to have been designed/drawn by hand on paper due to the lack of perfect geometry, spacing, and slight width variances of the traces, and the traces are full of curves. DXF turns curves into ugly polygons, like in my screenshot above. Does the Gerber format itself support bezier curves? And if so, which Gerber software has a bezier tool?
Also, I'm getting tons of DRC errors, like hundreds or thousands of them, all on the pads and traces. They are all "gap" related. The most common one is "Gap=0 mm; Rule=152mm". I have no idea what "gaps" they are referring to. There are no "0 mm" gaps between anything in the design (which would mean things were touching):
(https://www.eevblog.com/forum/eda/is-there-any-pcb-design-software-that-will-allow-me-to-use-an-image-as-a-guide/?action=dlattach;attach=274436)
This is what the original Illustrator file looks like:
(https://www.eevblog.com/forum/eda/is-there-any-pcb-design-software-that-will-allow-me-to-use-an-image-as-a-guide/?action=dlattach;attach=274438)
-
Also, I'm getting tons of GRC errors, like hundreds or thousands of them, all on the pads and traces. They are all "gap" related. The most common one is "Gap=0 mm; Rule=152mm". I have no idea what "gaps" they are referring to. There are no "0 mm" gaps between anything in the design (which would mean things were touching):
Yes, I have noticed this even when designs were initiated natively in DipTrace itself.
I'm not sure at this stage if it is a full blown bug or if it is caused by some setting (that I can't locate).
It pops up a lot when using copper planes & copper polygon fills.
I simply turn off the top layer & carefully look for for the red design rule error circles. If everything looks fine, I simply ignore the errors & successfully send the Gerber plots to the board house.
If anyone else has some ideas as to why this is occurring on DipTrace, please post. Thanks.
-
I tried it (Illustrator CS4 and pdf2gerb 1.6, which seems to be the latest version), and the output files were garbage.
A PCB like this, is getting outside their test-coverage, so I'd suggest starting with a design similar to their examples, while you establish the tool flows. Then, push things a little and see what is possible.
Does the Gerber format itself support bezier curves? And if so, which Gerber software has a bezier tool?
No.
Gerber files originally based on photoplotters, which are XY beds with motors, and a Lamp, and an aperture disk.
This stuff is very old, so does straight lines only. Any 'curves' are generated as polylines.
Likewise, lowest-common denominator translators, will also tend to use simple line segments, to give the best yields.
Of course, that safe/lowest level choice can be a pain in the details, as you have found.
Also, I'm getting tons of DRC errors, like hundreds or thousands of them, all on the pads and traces.
If you are starting from a polyline base, I'd pretty much expect DRC errors, as DRC scans for lines too close.
What makes touching line segments pass, is when the lines have the same net names.
That NET name comes from a Schematic flow, and here, you have no schematic flow.
-
I tried it (Illustrator CS4 and pdf2gerb 1.6, which seems to be the latest version), and the output files were garbage.
A PCB like this, is getting outside their test-coverage, so I'd suggest starting with a design similar to their examples, while you establish the tool flows. Then, push things a little and see what is possible.
Well, if the Gerber format doesn't support bezier curves, then there is no advantage to this Perl script method compared to importing a DXF anyway. The only reason I tried it was because I hoped it would preserve Illustrator's bezier curves.
No.
Gerber files originally based on photoplotters, which are XY beds with motors, and a Lamp, and an aperture disk.
This stuff is very old, so does straight lines only. Any 'curves' are generated as polylines.
How were PCBs with traces that have smooth analog-looking curves manufactured in the first place? This one I'm working on right now is based on the PCB in a Nintendo Entertainment System controller; I've modified the layout somewhat to work with a different video game system. But anyway, not only are the original traces full of smooth curves, but they look like they were drawn by hand and transferred to the PCB, like what would happen with a photosensitive stencil process, as is used in screen printing or PCB etching that you can do at home.
(http://i.imgur.com/If8xzlN.png)
See how hand-drawn that looks? The traces are nominally 0.5 mm wide, but that varies (I'm not talking about intentional width variance for handling different levels of current), and the geometry is very un-computer-like. Those curves which are lined up in a row have very mismatched radiuses, unlike what you would get with an "offset path" function in a vector program. That PCB was designed no earlier than 1985, and Gerber files were the usual method by that time, weren't they?
Here's another curvy trace PCB:
(http://i.imgur.com/9bTxcDJ.png)
That's from a Fisher snow plow joystick, which is still in production.
If you are starting from a polyline base, I'd pretty much expect DRC errors, as DRC scans for lines too close.
What makes touching line segments pass, is when the lines have the same net names.
That NET name comes from a Schematic flow, and here, you have no schematic flow.
Okay, so are those DRC errors a real problem for a PCB manufacturer, or can I ignore them?
-
No.
Gerber files originally based on photoplotters, which are XY beds with motors, and a Lamp, and an aperture disk.
This stuff is very old, so does straight lines only. Any 'curves' are generated as polylines.
How were PCBs with traces that have smooth analog-looking curves manufactured in the first place?
Long,long time ago, there was black tape, IIRC done 2x or 4x scaled, and then photo reduced on large cameras.
Google finds this
http://www.pcbwizards.com/handtape.htm (http://www.pcbwizards.com/handtape.htm)
'Bishop tape' could produce curves as shown.
Rubylith was also used, but less for curves, as that used scapel and drawing arms.
Okay, so are those DRC errors a real problem for a PCB manufacturer, or can I ignore them?
If you have no NET names, just use your eyeball check to confirm you are ok.
Addit: You could look at adding NET names manually.
The NET info is not complex, and some EDA tools will work-backwards to merge a polyline with the Pin-based NET info.
It also gives you a means to check the design, and should allow better DRC use.
-
Well, if the Gerber format doesn't support bezier curves, then there is no advantage to this Perl script method compared to importing a DXF anyway. The only reason I tried it was because I hoped it would preserve Illustrator's bezier curves.
Yes and no. A key advantage of the Perl Script, is you can avoid any other CAD tool, and use only Illustrator.
This one I'm working on right now is based on the PCB in a Nintendo Entertainment System controller; I've modified the layout somewhat to work with a different video game system. But anyway, not only are the original traces full of smooth curves, but they look like they were drawn by hand and transferred to the PCB, like what would happen with a photosensitive stencil process, as is used in screen printing or PCB etching that you can do at home.
Another reason for the demise of flowing curves, is the new EDA tools with Shove Routers make PCB design a lot easier, and Shove Routers tend to think at 45' increments. Most I've tried have a real distaste for any manually-added curves...
-
Yes and no. A key advantage of the Perl Script, is you can avoid any other CAD tool, and use only Illustrator.
I would still need to open the output files in something to verify that they are usable. With the DXF-import method I'm not using other CAD tools for anything other than compiling the PCB layers and generating the Gerber files. Well, ideally that's the case anyway. As it stands, DipTrace won't accept imported DXF drill holes so I have to add those from within the program. I noticed that Cadsoft Eagle can import DXF files too; I might see if it does any better with importing drill holes.
-
Yes and no. A key advantage of the Perl Script, is you can avoid any other CAD tool, and use only Illustrator.
I would still need to open the output files in something to verify that they are usable. With the DXF-import method I'm not using other CAD tools for anything other than compiling the PCB layers and generating the Gerber files. Well, ideally that's the case anyway. As it stands, DipTrace won't accept imported DXF drill holes so I have to add those from within the program. I noticed that Cadsoft Eagle can import DXF files too; I might see if it does any better with importing drill holes.
There seems to be some issue with importing holes in the current version of DipTrace... Let me have a play tonight and see what's up.
Also, DXF does support splines, however DipTrace doesn't support that version of the DXF standard. To get around it, use "dxf_s: -splineaspoly" as the pstoedit CLI option. That will convert splines to polys with reasonably good precision.
-
Yes and no. A key advantage of the Perl Script, is you can avoid any other CAD tool, and use only Illustrator.
I would still need to open the output files in something to verify that they are usable.
True, but there are plenty of Gerber Viewers out there.
KiCad has a reasonable one, which can also export to KiCad.
I'll check how that handles Drill....
Addit: Hmm.... well, that does do Gerber -> KiCad, with some caveats....
* PCB traces come in ok on a per-layer basis
* You can export Drill info to a user layer, so you can see holes and slots
* It seems to sense trace ends, and export as VIA, with a round diameter == Pad length. Drill is always 0.4mm
Caveats:
-- Vias do have drill (0.4mm), but alas not derived from the Drill-imported
-- Vias are placed on all PADS, including SMD ones.
-- KiCad Vias I think cannot change from Round, nor manually set Drill = 0.0, or separate layer stack-ups.
I guess that means for a Thru hole PCB, with no SMD, and only round pads, this could work.
One weird thing is slotted oval holes at 45' (ie the most complex) seem to convert ok, but the simpler SMD pads all morph to round ?!
Ahh.. seems flashed items are treated specially, different from drawn.
Flashed to F.Cu or B.Cu flip to Vias, Flashed to drawing layers flip to Round == H Value of Flash, no drill.
With the DXF-import method I'm not using other CAD tools for anything other than compiling the PCB layers and generating the Gerber files. Well, ideally that's the case anyway. As it stands, DipTrace won't accept imported DXF drill holes so I have to add those from within the program. I noticed that Cadsoft Eagle can import DXF files too; I might see if it does any better with importing drill holes.
Most CAD flows import DXF as for outline handling, and they design for portable first, so expecting to extract PAD stack and Drill information, is
maybe expecting too much.
If you want full information flow, you should be able to define PAD sizes on all layers, as well as Paste and Mask separately, and drill with plated/non plated choices.
I've not seen a generic DXF import go to that level, but I have requested that KiCad add a tool/macro to the Footprint editor, that can extract a circle or polyline, and generate a PAD definition or hole definition. - ie the simple footprint helper stuff.
The user would still need to select item, then select what to create, using that as seed.
Possibly, some layer names could be used to assist seed process, but with things like offset drilled oval pads, getting more automation would need more code - enough to scan for 'Drill-contained-within'
It is still technically possible to include PAD stack and Drill info in a DXF file, and Mentor for example, have two DXF export choices:
Flat DXF, which is close to a plotter, with no database structure - but it is highly portable.
Full DXF uses DXF comment fields etc, to tag entities so they can import back as PAD stack, Drill info outlines and rules etc.
This one is less portable, and often leads to complaints of clutter, for tools that ignore hidden attributes.
If you had control of the sources of both the EDA tool, and the DXF generator, you could, in theory, get a similar result.
-
a quick Google finds others have been before you ... look at this - PDF to Gerber is exactly what you want, as it also does the Holes, and manages solder mask and silkscreen...
http://swannman.github.io/pdf2gerb/ (http://swannman.github.io/pdf2gerb/)
pdf2gerb: Convert PDF to Gerber and NC Drill formats
Because the KiCad Gerber to KiCad seems to mostly work, I thought I'd try this pdf2gerb design set.
I grabbed https://github.com/swannman/pdf2gerb/raw/master/examples/pdf2gerb_example.zip
and loaded into Kicad.GerbView, and then used Export to PCB NEW button.
Below is the result:
Comments:
Seems to have managed Copper/Mask/Silk all ok, and has converted drilled pads to Via, but with the default drill of 0.4mm
This works here, because they are all round - Hard to tell if the original 10pin connector top right, was RND or Oval Pads ?
All the gerber viewers I tried, say round pads.
The supplied Drill.drd drill file, does import into Kicad.GerbView, but scaled wrong.(1/10th?) It seems to tag 0.6096mm and 0.5588mm holes.
- I'd guess a small fix to their script would fix that ?
KiCAD has a native file format that is simple ASCII, so a script that can do pdf2gerb, could be modified to do pdf2kicadpcb, and that probably could do a smarter job of drill and pad shape handling.
-
No.
Gerber files originally based on photoplotters, which are XY beds with motors, and a Lamp, and an aperture disk.
This stuff is very old, so does straight lines only. Any 'curves' are generated as polylines.
Technically, straight lines, circular arcs, and filled polygons. But that's about it if I'm not mistaken. The full gerber specification is very short and actually quite a nice read. Those who use gerber and haven't read it really should. Simple hacks like merging layers or adding "negative" patters to polygon fills is pretty straight forward =)
-
SprintLayout6.0 is the ticket for this job, and about 44.00USD.
-
I have used an image to recreate a board many times.
The old board is scanned in using scantocad which produced gerber or dxf, either will do.
These are imported into the cad software (CADSTAR in my case) as figures which will show me where pads and traces are supposed to go.
I create all the parts, draw the schematic and transfer that into this new board, place the components over the pads and then route it following the figures.
Having been party to also doing this on a 6 layer board with thousands of pins (luckily all PTH) where the outer layers had to be exactly the same this bit was relatively easy, figuring out the inner layer connectivity when not having a schematic was a tad harder and more time consuming but it wasn't impossible :)
-
For less than $50.00USD or 49.9 euro you can buy a fully licensed version of SprintLayout 6.0 that can do this easily. Just scan to a bitmap and float it in the background and trace over it with the program. You can do 2 layers at a time this way. Easy to learn, very short learning curve. In a hour or so you will be an expert.
You can also directly import 274X gerbers and turn them into a PCB quite easily. If you have the drill file for the 274X it will create the pad holes automatically. Works like a treat. I have converted CADSoft Eagle 274-X gerbers this way. It has a lot of power for the buck. You can download a fully functional program from their website (does everything but save).
I have made 100's of boards with this seemingly little known but powerful software.
It is amazing especially considering that the install is only a few megabytes! It can do things that P-CAD 2006 could not do but there are some limits:
1. No full auto-router (real PCB designers don't need one) :-DD
2. 4 copper layers
3. 1 outline/doc layer
There are workarounds for some of this.
No limit to the number of components or pins or anything crazy like that.
There are some videos available on YouTube. The ones by Juan Vargas are amazing.
Juan has also released a ton of Makros (that is what Sprint calls library parts) that can be found on the Yahoo! Sprint Layout Group
It is also stupidly easy to make your own parts.
Here is one of Juan's videos, he specializes in high performance audio design. An audio engineer's engineer for sure!:
https://www.youtube.com/watch?v=dtayIvORCWY (https://www.youtube.com/watch?v=dtayIvORCWY)
Good luck,
Sam
W3OHM
LeCroy Group Moderator and professional electron pusher
You can find it here:
http://www.abacom-online.de/uk/html/sprint-layout.html (http://www.abacom-online.de/uk/html/sprint-layout.html)
The usual disclaimer:
I have no financial or other interest in the company that makes this software.
-
if I wanted to recreate an existing PCB, the easiest way to do it would be to scan the PCB in at e.g., 600 DPI, drag the image into design software, set the opacity to about 50%, and then layout the PCB design on top of it, using it as a guide. When finished, the image can be deleted.
I have done EXACTLY that, in EAGLE, using the "import BMP" ULP program (and adjusting the image/scan/whatever it was I had to be the appropriate size, using an image editor beforehand.) (and then used the PCB to backtrack to a mostly-known schematic.)
(This was for the "Freeduino" project, and analysis/review/debug of the Solarbotics version, which had been done in a different CAD package.)
I've done similar things by importing gerber files (which is more directly supported), when I wanted stuff in a silkscreen layer that obeyed DRC rules as if it were copper (draw in copper, export layer using CAM to gerber, import gerber to separate layer, delete the original copper.)
I don't know if it's something that would work if you were trying to EXACTLY recreate an "artistic" layout, but it certainly works fine for using as a guide...
-
This was asked at the Kicad forums recently. In Kicad, you can make a "footprint" out of the PCB-layout image with the built-in "Bitmap2Component" module, then simply place components over the top of it & trace the routings etc. Then, obviously, delete the background footprint/image. You need to turn off the DRC check as you are not working from a prior schematic. It's easy & it works & there are no scaling/size issues with the background layout.