Hi all,
After a few months with KiCad 4.0.7 I switched to KiCad 5.0 and enjoyed the ability to import Eagle projects. Here is the outcome of my tests.
Intro: I work using a VM with Windows 10 x64 OS. I don’t have Eagle (not even the freeware version). I tested the feature by downloading the Eagle files and their PDF softcopies from a popular website with extremely good reputation.
-Import brd or sch does not seem to make any difference, I always end up with a KiCad schematic and PCB.
-Schematic looks exactly the same you see from the PDF softcopies from the source website. It doesn’t look exactly a KiCad schematic because it uses a library made of the Eagle components.
ERC shows a number of warnings about incorrect pin driving etc this is probably inherent to the schematic or to bad quality of library components. No fatal errors, though.
CVPCB is correctly populated and I sample tested a number of components, verifying that the viewers display correctly both the footprint and the 3D model.
No netlist is generated in the import/conversion process.
A netlist is generated without errors.
PCB: a pcb file is generated and shows a number of unrouted nets. Pressing “B” rebuilds the copper fills but after this there are still a few unrouted nets not easy to solve by hand without editing the existing tracks. Most of them are GND but I got also a couple of power supplies. Regardless of which nets are affected, I think that this should not happen at all.
I couldn’t find any settings to try in order to see if I can get everything routed as per the original files.
Thanks Rene.
I just did and ended up with the same result as pressing the B key (same residual not connected nets) plus a number of messages about “pad near pad” and “track near pad”.
I really would like to PM my files to you in order for you to have a look, please give me instructions for that.
Cheers
Due to the differences between KiCad and Eagle data, and differences in the fill algorithm etc, it will probably never be a 100% conversion for all cases.
Also, I converted Eagle projects from “a popular website with extremely good reputation” (Arduino) and the final project had errors not because of the conversion, but because of errors in the original project. So regardless, you will need to verify that the final projects are correct.
I did attempt to create a tool to compare Gerber outputs, but it wasn’t really practical.
Also Rene mentioned that there could be differences in the fill settings (or strategy as you say) so i posted in order to ask advice about different settings to try in order to see if this solves the issue.
But given your answer i will download the freeware version, which should be enough to handle the Arduino Due board i used for this test and look for errors in the original project.
Unless I missed something in your post, you haven’t looked at the original Eagle board to see whether these issues exist there. If you would like to post a link to the popular website with extremely good reputation, we can look at the conversion and see if there are issues to be addressed in KiCad.
That said, we are not able to provide 100% accurate conversion. The tool exists to help users adapt existing Eagle work. As @bobc says, there are different features that lead to slightly different results.
Hi Seth_h,
I tried to email the files to @Rene_Poschl , then got a reply from @bobc, so I believe that the files and the link arrived.
And yes, you missed (no offence!) that I highlighted that I currently don’t have Eagle installed.
Following Rene and bobc replies, I will install the freeware version of Eagle to check if the errors are in the original project or in the conversion.
The board is just the Arduino Due board, and its Eagle files can be downloaded from its page on the Arduino website: https://store.arduino.cc/arduino-due
Since I own a working Arduino Due board, I expect the Eagle project to be OK, but I never say never and will have a look.
Meanwhile, I kindly ask if someone can tell me how to alter the copper fill settings to try also this path to get a fully routed board without altering the imported files.
Hi Seth_h,
By comparing the Eagle imported schematic agains the PDF version on the website i found the error you mentioned. This explains the unconnected 5V on the PCB (see pic below)
Besides, i found also that labels USBVCCU2 and GND (pins 31 and 28 of IC6 resp.) are not placed correctly (see the endpoints of the 2 wires coming out from the chip?). Maybe this explains the unconnected GND nets?
Thanks
We move labels when they would otherwise connect to the wrong net in KiCad (Eagle labels are fixed based on association, not position).
The unconnected ground lines you see are issues with how Eagle interprets unlabeled nets (ignore) and KiCad interprets them (unique net). Because of this, the connection to the center of the pad where we connect the ground plane is broken by the overlapping drill hits that Arduino uses to denote a slot. Not much we can do about that automatically, that would be up to the user to identify what they want and make it in KiCad. In this case, you can delete the extra drill hits and change the hole shape to Oval in the pad properties
Nice to know. we had a question just yesterday from problems resulting from their workaround. Will need to find the original post again and update that there.
-in the schematic, by removing the extra junction between MISO and +5V at the upper R13 terminal the unrouted net is gone.
-in the PCB, by removing the extra drills and changing the last hole shape to Oval like @Seth_h said all issues are gone.
Final questions:
About the 5V unrouted net, @Seth_h wrote “This is a definite error in the import”.
Have i got to file for a bug report (no idea how to do that) or will you take care of it?
Or is it something that can happen so bottom line is to always double check what has been imported?
Thanks
