Author Topic: 20 Years with Ultiboard ... What Next?  (Read 18600 times)

0 Members and 1 Guest are viewing this topic.

Offline benst

  • Regular Contributor
  • *
  • Posts: 52
  • Country: nl
Re: 20 Years with Ultiboard ... What Next?
« Reply #25 on: February 16, 2018, 03:39:04 am »
Replying to an old thread here...

I have also been using Ultiboard since 198x on DOS and then Windows. I quit the support contract some few years ago because I felt it was worth it. Not many new features and 20+ years old bugs still unresolved.

Anyways, thinking of using KiCad from now on. Is there some form of conversion from Ultiboard/Multisim pcb+schematics to Kicad available? A quick duck-duck-go search didn't turn up anything useful.

Thanks,
Ben
I hack for work and pleasure.
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 12609
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: 20 Years with Ultiboard ... What Next?
« Reply #26 on: February 16, 2018, 03:56:25 am »
I'm not aware of any way to  convert the files to any other format, outside of the "analog hole" -- import netlist and gerbers.  Not that that's much help at all, since gerbers are flattened graphics and do not contain EDA objects.

Tim
« Last Edit: February 16, 2018, 04:00:56 am by T3sl4co1l »
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline benst

  • Regular Contributor
  • *
  • Posts: 52
  • Country: nl
Re: 20 Years with Ultiboard ... What Next?
« Reply #27 on: February 16, 2018, 10:19:09 am »
Ok, thanks. Was hoping for something better...

Ben
I hack for work and pleasure.
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 12609
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: 20 Years with Ultiboard ... What Next?
« Reply #28 on: February 16, 2018, 12:55:43 pm »
If someone wants to try and reverse engineer the format, they could stand to become slightly internet famous I think.  There's probably enough designs out there that one could stand to make a bit of money doing conversions.

It may not be too bad, but I don't have the tools to analyze binary compressed files.  (In case you're wondering, no, it doesn't open in 7zip.)

Tim
« Last Edit: February 16, 2018, 12:58:44 pm by T3sl4co1l »
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline Epaperman

  • Contributor
  • Posts: 5
Re: 20 Years with Ultiboard ... What Next? GERBERS
« Reply #29 on: August 29, 2018, 12:15:27 pm »
Here a tip for Ultiboard (DOS) users.

I am still using 4.84 April 1996

I tried the JCL PCB like Dave done in this video recently..

But Ultpost only can make Gerber RS-274D and not RS274X.

I found a way to make the pcb manufacteres happy..
I addded a amperture create table in front of the old gerber data.

"%ADD10C,.50*%"
"%ADD11C,.60*%"
"%ADD12C,.70*%"
"%ADD13C,.80*%"
"%ADD14C,.90*%"
"%ADD15C,.100*%"
etc

They can now read mt "old" gerber.. and currently producing my PCB.

 

Offline mairo

  • Supporter
  • ****
  • Posts: 122
  • Country: au
Re: 20 Years with Ultiboard ... What Next?
« Reply #30 on: February 22, 2019, 09:57:54 am »
I wonder if NI engineers use Ultiboard for theirs PCB designs now they own it?  ::)
 

Offline Doctorandus_P

  • Frequent Contributor
  • **
  • Posts: 536
  • Country: nl
Re: 20 Years with Ultiboard ... What Next?
« Reply #31 on: February 22, 2019, 01:14:46 pm »
I've also been using UltiBOARD from. quite long ago.
I bought it twice. First the DOS version, and later a Windoze version.

After some time you found ways to work around most of the bugs.
Of the Windows version they even kept sending me CD-Roms together with ever increasingly redicilous bills.
More then half of the CD-versions they send me crashed within an hour of starting them.
They really made me feel like a beta tester instead of a PCB designer.
Instead of fixing bugs their main priority seemed to be to desgin more bugs into the program.

An acquance of mine hade a cracked verson of the followup of that program, 10+ years later.
If you dared to drag a schematic component with 10+ wires attached it redrew all wires in random order and even made cross connections between those wires before it gave up. It was a horrible mess, and if Ctrl+Z didn't work you may spend 15 minuts on cleaning that up.
 So I snickered when I read:
Not many new features and 20+ years old bugs still unresolved.

After trying many different PCB programs I finally settled on KiCad.
KiCad has it's rough edges, but it's working pretty well for me. It is without doubt the best PCB progam I've ever used and I've tried to use about 10 low budged programs. Once I even paid EUR125 for "EdWin", that was EUR 125 down the drain.
KiCad is also rapidly improving. Don't put too much value into a 5 year old KiCad review!

Anyways, thinking of using KiCad from now on. Is there some form of conversion from Ultiboard/Multisim pcb+schematics to Kicad available? A quick duck-duck-go search didn't turn up anything useful.

I was curious about that so I had a look.
File import/export is a very immature funcionality at the moment in KiCad, but I know that Pcbnew (PCB part of KiCad) can export layers (Copper, silkscreen, or any other) as an SVG file, and it can import layers from a .DXF file. Weird combination, but it's probably on the roadmap to improve that. My curiousity was what you can do with GerbView (Gerber viewer part in KiCad).

As preparation I first made some Gerber files with KiCad of a very simple design I had liing around (2 diodes connected in parralell).
Imported all the layers in GerbView, and then I saw in the File menu an option for: "Export to PCBnew" so I tried that immediately.

It "Works" (partially).
In GerbView you first get a popup with how to export layers, and where to.
The Gerber format is pretty limited. It does not know the difference between copper and silkscreen.
It does not know what text is.

So I did the export in Gerbview, and imported it again in Pcbnew.
Board outline is recovered.
Traces are recovered.
Pad locations are recovered (but SMD pads seem to be converted to holes)
Silkscreen gets recoverd, but all silkscreen text is converted to individual line segments.

With the current state of KiCad (V5.0.2) the most sensible path seems to be:
- Redraw the schematic (Which is a nuisance, but redrawing a schematic is not that much work from even a paper printout.)
- From the schematic you can generate a normal netlist & footprint association.
- Use GerbView to export the board outline and copper traces to a KiCad project.
- Use GerbView to export the silk screen to a user drawing, fabrication or other auxilary layer.
- (You could even park notes on a unused copper layer if you deemed it usefull).
- Place the Footprints on the right places on top of the from Gerbview imported copper tracks.
- Do DRC for finding conversion errors, etc.
- Do some cleanup. You could for example double check the newly generated silkscreen text with the recovered lineart.

It's quite an labour intensive conversion this way, but it sure is a lot better than  completely redrawing a whole PCB from scratch, unless of course, the original PCB was designed badly. In that case you might as well start from scratch.

One of the improvements in KiCad V5 is that you can now handle copper tracks pretty much as line art just as any other grapics program would. The Net that a piece of copper belongs to, automatically changes if it is connected to another net, as long as it is only connected to one net at a time. This makes it trivial to copy a set of copper tracks to duplicate a part of a layed out board. Placing the right components on the copied copper tracks I still did manually. There are scripts for duplicating (parts of) a design in KiCad, but I have not tried to use them.
 
The following users thanked this post: benst

Online nctnico

  • Super Contributor
  • ***
  • Posts: 16532
  • Country: nl
    • NCT Developments
Re: 20 Years with Ultiboard ... What Next?
« Reply #32 on: February 22, 2019, 11:22:50 pm »
In my experience it is quicker to just redraw the traces as well. 90% of a board layout is component placement so if that has been done, drawing the traces only takes a little bit of extra time.
There are small lies, big lies and then there is what is on the screen of your oscilloscope.
 

Offline Doctorandus_P

  • Frequent Contributor
  • **
  • Posts: 536
  • Country: nl
Re: 20 Years with Ultiboard ... What Next?
« Reply #33 on: February 23, 2019, 04:47:47 am »
If you have all the trace ends from the Gerber output, you do not have to think about component placement, you simply put them back over the existing trace ends. No need to nudge or move components afterwards to make room for routing races.

The "90%" that goes into component placement, is not in the places the compents are but in the thought process that results in the final component placement. This makes reprocuction from an example a lot faster, then re-inventing a new component placement from scratch.

Somewhere between 40% and 70% seems more realistic between component placement and routing.
The info KiCad can easily recover from a Gerber file is worth the few mouse clicks of effort.
Just the board outline, mounting holes and connector placement is worth it.

And by simply putting the components back where they were you get (most of?) the routing for free from the backport of the Gerbers.
Backporting the Gerbers is a 5minute effort and it can easily save half an hour upto several hours of effort of re-creating the board outline, component placement and routing.

Here is a story about routing a fairly complex design in KiCad. If a project with that level of complexity had to be re-created from documentation, then being able to backport from the Gerbers would be a very significant benefit. At Purism they say it took them a month to get the routing right.
https://puri.sm/posts/how-we-designed-the-librem-5-dev-kit-with-100-free-software/
« Last Edit: February 23, 2019, 05:11:19 am by Doctorandus_P »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf