| Author |
 Topic  |
|
|
Chris55000
United Kingdom
38 Posts |
 Posted - 02 May 2024 : 08:54:33
|
Hi!
I am trying to make a PCB for the British Amateur Television Club's PAL Encoder circuit from three decades ago, and I am running into numerous problems with EPC V27.0.1 which are :–
a) Both the Schematic and PCB D.R.C.'s report dozens and dozens of "Empty Nets" using Net Names from numerous previous designs along with many "missing components" – the board design I am trying to complete consists of 86 resistors, 29 capacitors, one axial inductor, two diodes, one zener,15 bipolar transistors,ten presets, one TTL and one linear device, all basic through–hole devices!
I am getting countless errors related to Net Names "A0–A15, __IRQ", etc., etc., that all relate to a previous board I did for my friend three years ago!
b) Neither forward now back annotation will work, and the "Reverse Engineer" caused a major crash that results, each time, in the software having to be completely uninstalled using "Revo Uninstaller" and then completely reinstalled before Easy PC will run again ;
c) Attempts to use the "Translate to PCB" don't work – I plotted the board layout (of components) completely manually using the original B.A.T.C. sketch – can you not use "Autoroute" tools on a manually placed board ?
d) I did plot a complete "Easy PC" schematic from scratch for the design I'm trying to create, but that hasn't helped either!
e) I am still getting a repeated problem of net–names sticking with each new track I attempt to route, causing multiple short–circuits over large sections of the design, and neither "Change Net" or "Disconnect From Net" resolves the problems, and even when I plotted a new schematic entirely from scratch, the same thing is still happening on the Schematic – this HAS to be an unfixed bug somewhere, it is happening on virtually every design I attempt to make with this software!
. . .I can email the files if need be, and I have had permission from the B.A.T.C. to re–create old board designs for research/study purposes!
Chris Williams |
Edited by - Chris55000 on 02 May 2024 09:07:58 |
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 02 May 2024 : 09:07:17
|
Go to your nets lists and "Delete unused nets"
Iain |
 |
|
|
edrees
United Kingdom
779 Posts |
Posted - 02 May 2024 : 09:40:37
|
It appears you have "artifacts" from previous designs. After deleting unused nets (Design Tech=>Nets=>Delete Unused) on BOTH schematic and pcb run a "Design Rule Check" on your Schematic and then "Forward Design Changes" to the pcb. They should then be in "sync", - confirm by performing a Tools=>Integrity Check in pcb editor.
Take backups of everything beforehand, -just in case!
|
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 02 May 2024 : 10:48:41
|
You mentioned that you can't forward changes. In the pcb design, go to [Tools], [Back Annotation] and use the [View Renames] button. If you're happy that these changes don't need to be done to the schematic then you can use the [Delete Renames] button to clear the list. If they're relevant then you just back annotate. Either way, the list will be cleared, allowing you to use Integrity Check and Forward Changes.
Especially in the schematic, many of the design rule check options are warnings rather than errors. When you're in the DRC setup dialogue, press <F1> for more information about what each option does.
If you're repeatedly getting a lot of nets included from previous designs, you may need to edit the technology files used to create those new designs. You can open technology files using [File], [Open] as with designs, then you can check on any retained parameters like net names and value names using the same design technology menus as you would in a design. With existing designs, if you go to [File], [Properties] you can discover the technology file used when the design was created.
|
|
|
|
Chris55000
United Kingdom
38 Posts |
Posted - 02 May 2024 : 13:11:19
|
Thanks Gents!
I'll look at all those points and check them on all my previously completed designs – it's something that needs to be explained in the User Guide to draw users' attention to – I wonder if a grotesquely long list of net names that Easy PC has hoovered up and saved from previous designs is responsible for the crashes?
Note for the Programmers – could a simple "Design Maintainence" automatic utility/toolbar button not be designed that does this, with a suggestion in future revisions of the User and Evaluation Guides to use such a facility before starting each new Schematic and PCB design?
Chris Williams
|
Edited by - Chris55000 on 02 May 2024 13:17:20 |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 02 May 2024 : 13:18:43
|
| I tried sending you a personal email but the address bounced. Can you please send details of your proposal to <support@numberone.com> as that will get the programming team's attention. Thanks. |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 02 May 2024 : 13:43:02
|
| Chris, - did we used to work together in the 1980's at Winnersh? |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 02 May 2024 : 16:13:26
|
| Easy-PC files are encrypted to protect against hacking. This is obviously transparent to users but will probably prevent import by any other software unless a technology sharing agreement is in place. As far as I am aware, this does not include KiCAD. |
|
|
| |
Topic |
|
Problems with "Empty Nets" causing multiple errors