20 Years with Ultiboard ... What Next?

[T3sl4co1l]

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

[benst]

Ok, thanks. Was hoping for something better...

Ben

[T3sl4co1l]

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

[Epaperman]

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.

[mairo]

I wonder if NI engineers use Ultiboard for theirs PCB designs now they own it? 

[Doctorandus_P]

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.

[nctnico]

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.

[Doctorandus_P]

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/

[Jeroen3]

Reading this seems like there is no migration path at all to anything else if you are on Ultiboard, which is unoficially retired by NI. (Last version 5 years ago)

Is this still correct in 2019?

Altium Circuit Studio pricing is very attractive, but the volume of old designs seems to be holding back the company.
There is no component library of sorts at all. Since this is something Ultiboard does not support properly on >Win xp.

What would be the best step forward, away from the funny business and unreliability of NI?

[EEVblog]

I'd just move to KiCAD unless you have some specific requirement.

[nctnico]

Reading this seems like there is no migration path at all to anything else if you are on Ultiboard, which is unoficially retired by NI. (Last version 5 years ago)

Is this still correct in 2019?

Altium Circuit Studio pricing is very attractive, but the volume of old designs seems to be holding back the company.
There is no component library of sorts at all. Since this is something Ultiboard does not support properly on >Win xp.

What would be the best step forward, away from the funny business and unreliability of NI?

If this is for professional use then look at Orcad (with CIS option) or Altium. You'll need a package which has a good solution (=support for a component database) to deal with the logistics side of producing boards. Feature wise Orcad and Altium are about equal however Orcad has lower hardware requirements for the PC it runs on.

[Jeroen3]

The company is not involved in high density or complex boards. Up until now all of them are 2-layer and the smallest part was a 0402 cap. It's more power electronics, so not much high density.
I see that Orcad includes simulation, that might help convincing some people. Not a large team though, 4 people.
If the software can take over some of the burden of project logistics it might save a lot of time. Now all part management is manual.

I see KiCad has improved a lot since the last time I checked. Will definitely check this out for a project at home.

[nctnico]

The company is not involved in high density or complex boards. Up until now all of them are 2-layer and the smallest part was a 0402 cap. It's more power electronics, so not much high density.
I see that Orcad includes simulation, that might help convincing some people. Not a large team though, 4 people.
If the software can take over some of the burden of project logistics it might save a lot of time. Now all part management is manual.

You don't need to make complex boards for Orcad or Altium to pay off. The way I have been working with Orcad for the last 20 years is as follows: I have a database which has a part description, manufacturer, manufacturer part number, part value, schematic symbol, PCB footprint (nowadays one for Orcad Layout and one for Allegro), budgetary prices, my inventory (stock) and order codes from Farnell and RS. Added to that every part has my own internal part number which is the database key. My Orcad part libraries are symbols only. They do not contain any information about manufacturer, values, footprints, etc. This means that I have one symbol of a resistor. A component in a schematic links to my part number. For example: if I want to change to a different resistor symbol I do this in the database and then update the schematic. Ofcourse time needs to be spend on adding parts to the database but being able to re-use a part pays and knowing that an existing part is correct pays off quickly. When I create a BOM for a board I have to press one button the create an Excel file which has all the right part values and manufacturer part numbers. It can go straight to an assembler. Or when I build a prototype I can use the inventory information to see which parts I need to order (using the order code) and which I have in stock. Altium has a similar workflow using an external database.

KiCad OTOH does not have something like this. You'd have to create multiple copies of the same symbol to have different values. This gets tedious quickly because you don't have the overview and flexibility a database allows. If you make a mistake in a BOM then things can get costly quickly just from time spend looking for where the problem is in a circuit. The more you automate part management the less errors you have.

[Bassman59]

KiCad OTOH does not have something like this. You'd have to create multiple copies of the same symbol to have different values.

That is not true.

[Jeroen3]

I read about the KiCad library convention, and they appear to have copied what eagle does. Symbols that you can attach to any number of Footprints.
Or more the other way, footprints you can link to symbols.

[nctnico]

KiCad OTOH does not have something like this. You'd have to create multiple copies of the same symbol to have different values.

That is not true.

If that is the case then show us how you can use an external database with component information together with Kicad where Kicad uses the information from the external database to keep the component information up-to-date and create bills-of-materials. Last time I checked Kicad wasn't able to do this and there was not even a roadmap to integrate a feature like it. IMHO that is a pity because it is the only feature missing which would put Kicad on par with the big guys.

[Bassman59]

KiCad OTOH does not have something like this. You'd have to create multiple copies of the same symbol to have different values.

That is not true.

If that is the case then show us how you can use an external database with component information together with Kicad where Kicad uses the information from the external database to keep the component information up-to-date and create bills-of-materials. Last time I checked Kicad wasn't able to do this and there was not even a roadmap to integrate a feature like it. IMHO that is a pity because it is the only feature missing which would put Kicad on par with the big guys.

I have a master parts list database. All of my library parts have house part numbers. For things like resistors and capacitors, you place a generic symbol on the schematic and change the value to whatever you like. Then a script takes the BOM from Kicad and creates a BOM with orderable part numbers. For those resistors, the script takes the house part number and the value and looks up that orderable part number.

I'm sure others use a similar system.

But what I find interesting is there are people who demand that the Kicad developers implement such a system, but those demands are never followed up with any proposals on how to do it or offer to start implementing it.

That's not to say that a database-driven parts library would be a bad idea. I think everyone would love to see one. Someone needs to step up.

[nctnico]

I did contemplate on hiring someone to implement a database driven component system into Kicad but my past experiences with contributing to open source projects have made me decide not to go that route. Added to that is that the whole library system was in a state of flux at that time. Maybe CERN will pony up the money / resources at some point.

I used to use scripts / external programs too to create bills of materials 20 years ago. I don't want to go back to that time. It is still very prone to errors. Orcad for example can run a check to verify all components against the information in the database.

[MarcV]

Funny to read that so many people are still using the old Ultiboard. I too have been using Ultiboard since the early nineties and am still stuck at version 5.72 for Windows. Actually I'm not even planning to switch to something else. It's just too difficult to switch when you think like the program does.

At some point it became difficult to find a working PC with a parallel port to connect the dongle to. So I decided to have the dongle "virtualized" by some obscure company on the web. But this works and I am now running Ulticap and Ultiboard on Windows XP inside a virtual machine.

By the end of the nineties I wrote a little tool to convert Autocad DXF files into Ultiboard component outlines. It was a very simple tool that only accepted simple lines, arcs and circles. An early version of that tool was also included on the Ultiboard CD Rom. In 2016 I decided to give that tool a complete makeover. The new tool allows you to draw a complete component shape including pads in Autocad or another program that can export DXF files, and import that DXF as a shape in your Ultiboard design file. The tool can interpret single lines, polylines, lwpolylines, arcs, circles and ellipses (which are automatically converted to line segments). Splines are not supported but can easily be converted to plines in Autocad. Pins/pads are defined as blocks with parameters in the DXF drawing.

These days shapes of components are usually made available in the 3D step format. I import the model in Autocad where it is flattened and saved as a 2D shape. The result is usually a highly detailed 2D drawing, much more than can be handled by Ultiboard. The new tool is capable of optimizing the data from the DXF output. A component shape in Ultiboard can only contain 1000 vertices and 64 arcs/circles so it's a good thing to reduce data where possible!

The tool can not only import DXF files but it can now also export component shapes to DXF format. This makes it easy to copy a shape to another PCB design without the need to transfer pad sizes as this is done automatically with the DXF import.

Oh and there's a hidden feature... back in the days there also existed an Ultiboard version called "Ultiboard Studio". Files saved with this version could not be opened by the regular version. This was done by a very simple "invisible" encryption, by changing the case of some characters in the DDF file from upper to lower case. If you run such a file through the DXF converter, this encryption is automatically removed 

Screen shot of the DXF<>DDF converter...


Example of what a shape looks like in Autocad...

[cinderblock]

I hope this post on an old thread is ok.

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

I did this. Some basic observations of a few sample files made me realize it's packed, byte aligned, compressed data. The first few (ASCII readable) bytes even suggest it's "Compressed XML".

With some more internet sleuthing and awesome netizens that recognized the pkware compression headers, I was able to export the full "human readable" XML data of Ultiboard (and MultiSIM) files!

I'm hoping to also get a compressor working but that has been a lower priority.

In case anyone wants to see or comment: https://github.com/cinderblock/EWD

[benst]

With some more internet sleuthing and awesome netizens that recognized the pkware compression headers, I was able to export the full "human readable" XML data of Ultiboard (and MultiSIM) files!

I'm hoping to also get a compressor working but that has been a lower priority.

In case anyone wants to see or comment: https://github.com/cinderblock/EWD

Nice work! I was able to convert a small Ultiboard 12 PCB into XML. I used the wip branch, it looks like that one is the latest one?

The generated XML is quite verbose. I could recognise a few Refdes, Net names and other designators. I was also able to load the XML file back into UB12, and it looked the same.

It would probably be quite a lot of work to write a translator into KiCad.

Ben

[cinderblock]

Nice work! I was able to convert a small Ultiboard 12 PCB into XML. I used the wip branch, it looks like that one is the latest one?

Thanks! `master` branch should work but I'm moving to a different decompressor library in the `wip-*` branch because it also has (or will have) a compression function as well. I haven't had time to polish it up at all. Glad it worked for you!

The generated XML is quite verbose. I could recognise a few Refdes, Net names and other designators. I was also able to load the XML file back into UB12, and it looked the same.

Yeah, there will need to be another layer on top of editing these XML files probably. I could totally see certain manual edits breaking a lot of things. But now we can at least experiment!

It would probably be quite a lot of work to write a translator into KiCad.

Agreed. But one can hope!

[scopeman]

Replying to this old thread but Pulsonix can import those files.

Sam
W3OHM

[Pieter Smets]

I there any one on this forum who can sell me Ultiboard/Ulticap 1600pin DOS version with dongle?

Have some old work I want to look at and can't access any more because I lost my dongle. :-(

[spostma]

I still have (and use) the 1400-pin DOS version, and am happy to
convert your design to Gerber, TIFF, HPGL or whatever you want.

Even Postscript --> DXF I can generate for you.

I also can do small board corrections for you if you want.