I had heard of FutureNet Dash, but had never used it. It is the first schematic capture program usable for designing Xilinx FPGAs and maybe the first schematic capture program available for IBM PCs. Recently I discovered that a version is available online, but no manuals. These are my notes from learning to use this $3850 (1988) program.
Why even look at such an old program? Well the user interface of these pre-Windows programs is always interesting to explore. I'm familiar with "Old DOS OrCAD"- it still has an active community and competes well even with modern ECAD programs. OrCAD was the lower cost option for schematic cature, so I'm curious what the high-end tool was like.
Michael Holley wrote this about FutureNet (extracted from the Wayback Machine):
And contributed this some brochures and a price-list to bitsavers, here:
http://www.bitsavers.org/pdf/futureNet
Some ASICs used in the Atari ST were designed in FutureNet, see here:
https://www.chzsoft.de/asic-web/
"FutureNet DASH was a schematic capture program written for IBM DOS PCs released in the early 1980s. It was an extremely expensive package - over $5000 at the time. After passing through various hands the software was released as version 6.10 in a de-restricted version."
This is from Contrelec, which hosts this final version:
http://www.contrelec.co.uk/pages/dashcon
There is a review of it in the October 1983 issue of PC Magazine. This article mentions some old "mainframe" electronic design pacakges I will have to look into at some point:
There is no further documentation that I can find. However, the program has on-line help. I've extracted it here:
The commands are organized by function by prefix:
. commands are for symbols / parts
/ commands are for wires
# commands are for hierarchy
[ commands are for area cut and paste
' commands are for text
Commands with no prefix are for everything else, such as file operations.
You need to set up the environment. It's a good idea to create a batch file for this:
SET FNMOUSE=M
SET FNDISPLAY=C:\DATAIO\FN\VGA12.DG
SET FNLIB=C:\DATAIO\FNLIB
SET FNLOG=FNLOG.CMD
SET FNELOG=FNERR.LOG
SET FNPRO=FNPRO.CMD
path=c:\dataio\fn;%path%
Then type "fn" or "dash" to start the program.
These macros are assigned to function keys, so they are probably important:
F1 HELP
F2 QUIT
F3 'P
F4 'L
F5 /D Draw or delete a junction
F6 /ES Delete line segment
F7 /P
F8 /ET Erase temporary lines?
F9 '0
F10 /0 Cycle through line styles
Sadly, I can only get it work in 640x480 mode with the VGA12.DG driver in DOSBOX. The release notes mention higher resolution modes, but I think either the driver is missing or I'm missing information on how to select them.
OrCAD has a huge advantage here- the display driver architecture is documented and assembly language source code examples are provided. People have made drivers that work on recent video cards (it works well in DOSBOX) and have even created a GDI driver that allows you to have a resizable window up to the size of any modern display supported by Windows. OrCAD is still a DOS program, so only 32-bit versions of Windows will run it. The lack of virtual-8086 support from 64-bit mode processors has forced OrCAD users to turn to DOSBOX. Unfortunately this is step back compared with how it worked with the GDI driver.
Normally you are in "graphic editing" mode. From this mode, you can type commands. Note however that if you hit Esc, you enter "alphanumeric" mode. Hit Esc again to return to graphic editing mode.
From graphic editing mode you may type in a command. When you press Enter, the command may prompt you for futher missing information. Once all information is provided and you hit Enter, the command executes.
Interestingly, the command line doesn't clear after you hit Enter- instead the last command line is retained so that you may hit Enter again to repeat the command. Only when you start typing a new command does the line clear.
You can actually enter a small script at the command line: multiple commands may be entered, separated by semicolons. Again it is retained, so hitting Enter repeats the script.
Scripts may be bound to keys with the KEY command. You can execute scripts saved in files with the AUTO and EXEC commands.
By contrast, OrCAD does not have a command line, instead there is a keystroke-based menu system: You hit 'P' for the placement menu, and then 'T' to place text. You can hit 'R' to repeat the previous single command. There are keyboard macros and you can start recording with the 'M' command and then by selecting which key you want the macro to be bound to. There is also a text form of these macros which can be bound to keys in a setup file. There is no way to execute a script file, but in one way OrCAD macros are more powerful: you can hit Ctrl-Home during recording at any point requiring user input. FutureNet has no such feature, but will automatically assume "Yes" to any Yes/No questions that commands may have.
You can move the cursor with the mouse, but also with the keyboard. Arrow keys will move the cursor, as well the "left", "right", "up" and "down" commands.
You can enter a repeat prefix before hitting an arrow key. For example, 5 then right-arrow moves 5 positions to the right. The prefix is retained for additional arrow key presses.
The repeat prefix does not seem to work as a command: you can not say "5;right" for example.
The displayed screen is a small window onto the larger schematic sheet. As with OrCAD, FutureNet uses auto-panning. It means that if you hit the edge of the screen with the cursor, the screen automatically pans in the given direction to view more of the sheet. FutureNet displays scrollbars, but there is no reason to use them.
It's difficult to convey just how much more conventient and quick this is to use vs. scroll bars, though I think it works better in OrCAD somehow- sometimes FutureNet doesn't detect the pan request.
There are commands to control the displayed grid:
grid - Turn the grid on or off
grid n - Set grid factor
grid snap - Turn snap-to-grid on or off
I've found that you probably do not want snap-to-grid on. Many symbols have pins which are not aligned with the displayed grid. Also the native grid is not much finer than the displayed grid, so you don't really need it.
In OrCAD you always want snap to grid, since the native grid is one pixel.
Having all key symbol points on a grid is very important for keyboard acceleration. You can make commands (or macros in OrCAD) to lay down a series of wires or labels in a structured way. This is basically impossible to do without a grid.
The finest grid looks like this. At this level you will find that everything is on the grid.
There is a command:
size a Select A size sheet
The default size is b.
An annoying limitation is that you can not reduce the size of a non-empty drawing.
When you are in no other mode, right click to bring up menus of all available commands. I suspect this was added in later versions to keep up with GUI fads.
Hit PgUp and PgDn to jump between different magnifications. You can also use the "zoom" command for custom ones.
Zooming works fairly well in that a correctly scaled font is chosen for the zoom level. Well at least two of the prefined magnifications have legible text. OrCAD had only a single text-legible zoom level.
* <Part number> <Enter>
.L <Part number> <Enter>
* <Enter> - It will prompt for the part number
.L <Enter> - It will prompt for the part number
Single device per package parts are named as you would expect, for example use 8088 for an 8088 microprocessor. But for a TTL inverter, you need to use "7404A" to get the first one of the package, or "7404B" for the second one, etc.
OrCAD has the "G" (get part) command for this. You can type in the part, or scroll through a text-only list of them.
Left-click in the center of the part and it should enter move part mode.
Also you can type . M <Enter>
There are a number of commands for this:
.R Rotate part
.RE Reflect part
You may enter these command while a part is already attached to the cursor for moving.
Position mouse over part and enter . C <Enter>. A copy of the part will be attached to the mouse.
Position mouse over part and enter . E <Enter>.
Type .DIR <Enter>
A window with a list of symbol libraries along with a list of symbols and a preview pops up.
OrCAD also has a part browser with preview, but you have to step through parts one at a time. FutureNet's browser is definitely better.
You need to do this to make the symbols in a library available to you.
Type .LIB <Enter>
You will be prompted for the name of the library. You can enter a complete path, such as C:\DATAIO\FNLIB\GENERIC.LIB.
These are in SYSTEM.LIB, which seems to be loaded by default:
TBLOCKA, TBLOCKB, TBLOCKC, TBLOCKD, and TITL are title blocks.
TX1, TX2, TX3 are transformers.
SWNC, SWNO are switches.
RES is a resistor.
POT is a potentiometer.
PCAP is a polarized capacitor.
CON1, CON3, CON4, etc. are generic connectors.
DIODE is a diode.
JUMPER is a jumper
These are in GENERIC.LIB:
BULLETIO I/O port (inter-sheet connector?)
BULLETR (inter-sheet connector?)
CONnn Generic connectors
EGND Normal earth ground
GND1, GND2, GND3.. other grounds
E4 power?
Postion the mouse over a pin (valid pins are highlighted when you hover over them) and left-click (no need to hold) to start drawing. As you move the mouse, the potential line segment is shown as a dashed red line. Left-click again to solidify the segment and start a new one from the current position. To stop drawing, right-click the mouse.
Do not hit ESC to complete drawing- it switches to text mode. If you do this, hit ESC again to return to graphics mode.
You can also type / L <Enter> to start drawing a wire- I'm not sure why they have this since you can just left-click.
Use / d <Enter> or hit F5 to draw or delete a junction dot.
Position mouse on wire, then hit F6 or type / E S <Enter>.
FutureNet calls all text "Alphanumeric Fields". What the text actually does depends on where it is located and what its "attribute" is. I think we would call attributes types today. Attributes are mostly predefined (but there are also user defined attributes), and are numbered and named.
OrCAD does not have this attribute concept. Instead the type of any text depends on where it is located. Typically there are different entry methods for the different locations.
Anyway to place a label, first decide on the purpose of the text. For a label on a wire, we want a "SIG"- a Signal, which is attribute number 5. So enter the command to select this attribute:
'a sig <Enter> - Choose attribute by name
'a 5 <Enter> - Choose attribute by number
'a <Enter> - Brings up a menu of attributes
From now on any new "Alphanumeric Fields" we enter will be signals. In the rather likely event that you forgot to select the correct attribute type, you can change the attribute of existing text like this:
'ch a sig <Enter> - Change attribute of text under mouse to SIG
Now to actually write some text, position mouse on a wire and hit ESC. This switches to text mode and you can type the label. The "Point of Effect" (as FutureNet calls it) must be on the wire. When you are done typing, don't hit <Enter>. Instead hit ESC again to return to graphics mode.
There is a command 'd that reveals the attribute codes (somewhat like WordPerfect's "reveal codes")- all of the text is replaced is replaced by the attribute code assigned to it.
Here is sheet with a number of different types of alphanumeric fields:
After hitting 'd:
Position mouse on label and type
'E <Enter>
| Number | Name | Description |
|---|---|---|
| 0 | COM | Comment? |
| 1 | PIN | "40" pin number |
| 2 | LOC | "UNNN" reference designator |
| 3 | PART | "8088" |
| 5 | SIG | Signal (wire label) |
| 20 | PINT | "26" Tristate pin |
| 22 | PNBT | "9" Bidirectional pin |
| 23 | PINI | "33" Input pin |
| 24 | PINO | "24" Output pin |
| 50 | TITL | Title in title block |
| 51 | DNUM | "000000" Drawing number in title block |
| 52 | DREV | "A" Rev number in title block |
| 53 | DPAG | "1 OF 1" in title block |
| 54 | DATE | "July 26, 1991" Date in title block |
| 100 | GND | Auto-connect to power net (shows in lower right corner of 7404 symbol) |
| 101 | +5V | Auto-connect to power net (shows in upper right corner of 7404 symbol) |
OrCAD has a special power symbol and you give the name of the rail as the part value. FutureNet works differently: you label a wire with the name of the power rail and set the attribute of the label to "PWRS" (for "Named Power Signal").
It is common to have hidden and automatically connected power pins on 74xx series TTL gates. The symbols for such gates include pin numbers as two text fields (often pins 14 and 7). The attributes for these fields are "GND" (attribute 100) and "+5V" (attribute 101).
Questions: Are all attributes above 100 global? How do you have a hidden +3.3V rail?
Create a symbol for a subsheet by creating a "functional block". Use the .F command to create it. Within the functional block symbol, place an "alphanumeric field" containing the file name of the sub-sheet, with its attribute set to FILE (attribute number 8).
Point to the file name and issue the "#D" command (down hierarchy) to descend into it. You can issue the "#U" command (up hierarhcy) to return to the previous level. The first time you descend into a file FutureNet will indicate that it is new and ask if it should be created.
The functional block should include pins for the signals that are to be brought up from the subsheet. Create them with ".-". The pins should be labeled with text that has one of the pin attributes: PINI (for inputs), PINO (for outputs), PNBT (for bidirectional), etc.
The subsheet itself should have a wire labeled with text matching the pin. "SIG" works as the attribute for the text (and I suspect other attributes will also work).
OrCAD has dedicated module port symbols this.
Here is an example sheet with two functional blocks containing subsheets in it:
Here is the "source" sub-sheet:
Here is the "dest" sub-sheet:
The netlist ends up like this. 'q' and 'd' are gone, but the part are connected together with the top-level net 'mysig'.
(SIG,,+5V,,,
PIN,2-1,1,U1,101,14
PIN,3-1,1,U2,101,14
)
(SIG,,GND,,,
PIN,2-1,1,U1,100,7
PIN,3-1,1,U2,100,7
)
(SIG,,mysig,1,5,mysig
PIN,2-1,1,U1,21,3
PIN,3-1,1,U2,23,1
)
A single functional block can be made of multiple sheets, so one way is to create a top-level sheet with a single functional block (create with .F) in it. Within the functional block symbol, place multiple "alphanumeric fields" containing the file names of the sub-sheets, each with their attribute set to FILE (attribute number 8).
Point to the first of these and type "#D" to descend hierarchy. You can hit "#U" to return to the top-level. The first time you descend into each file FutureNet will indicate that it is new and ask if it should be created.
When you are in one of the subsheets, you can traverse between its siblings with the #R and #L commands.
Here is an example of this. This is the top-level sheet. The functional symbol has three sub-sheets names page1, page2 and page3.
Here are the sub-sheets:
Another way is to feed a list of top-level sheets to DCM.EXE when you build the netlist. You will not be able to use the #R and #L commands to traverse between sheets this way.
Either way, all of the sibling sheets share the same namespace for signals- two wires labeled with the same signal name will be connected.
In the example above, the netlist ends up like this:
(SIG,,+5V,,,
PIN,2-3,1,U1,101,16
PIN,2-2,1,U2,101,14
)
(SIG,,GND,,14,GND
PIN,2-1,1,R1,1,2
PIN,2-3,1,U1,100,8
PIN,2-2,1,U2,100,7
)
(SIG,,isel0,2,5,isel0
PIN,2-1,1,R1,1,1
PIN,2-2,1,U2,21,2
)
(SIG,,sel0,2,5,sel0
PIN,2-3,1,U1,21,15
PIN,2-2,1,U2,23,1
)
In OrCAD, you can supply an aligned vertical list of file names in a top-level sheel (not as part of a module symbol). Very old versions of OrCAD also supported having a list of file names in a text file, but this feature was deprecated.
OrCAD has an automatic annotation process to replace the default reference designators (such as U? in OrCAD or UNNN in FutureNet) with unique numbers (U1, U2, etc.). I have found no such thing in FutureNet. It seems you have to set them by hand.
I must be missing something here.
The sequence of commands is as follows:
First you preprocess the .DWG files into a single .DCM file with:
DCM -itop -lfirst+second -oout
The commnd line length is very limited in MS-DOS, so you may also provide all of the names in a text command file (this mimics the MS-DOS LINK command). In this case you invoke DCM like this:
DCM @list
The command file, list.cmd should look like this:
-itop
-lfirst
second
-oout
Next you convert the .DCM file into a FutureNet native .NET file with:
NETC out
The netlist looks like this (which looks extremely like the Xilinx .XNX netlist format):
NETLIST,2
(DRAWING,\TRYNET\TOP.DWG,1-1
)
(DRAWING,\TRYNET\SOURCE.DWG,2-1
PATH,\TRYNET\TOP.DWG,1,
)
(DRAWING,\TRYNET\DEST.DWG,3-1
PATH,\TRYNET\TOP.DWG,2,
)
(SYM,2-1,1
DATA,2,U1
DATA,3,7400
DATA,23,1
DATA,23,2
DATA,21,3
DATA,100,7
DATA,101,14
)
(SYM,3-1,1
DATA,2,U2
DATA,3,7404
DATA,23,1
DATA,21,2
DATA,100,7
DATA,101,14
)
(SIG,,,,,
PIN,2-1,1,U1,23,1
PIN,2-1,1,U1,23,2
PIN,3-1,1,U2,21,2
)
(SIG,,+5V,,,
PIN,2-1,1,U1,101,14
PIN,3-1,1,U2,101,14
)
(SIG,,GND,,,
PIN,2-1,1,U1,100,7
PIN,3-1,1,U2,100,7
)
(SIG,,mysig,1,5,mysig
PIN,2-1,1,U1,21,3
PIN,3-1,1,U2,23,1
)
You may convert the .NET file into a PADS ASCII file with:
NET2PADS (it prompts for the name of the .NET file)
PADS is a PCB layout program.
The netlist looks like this:
*PADS-PERFORM-V6-MILS* DESIGN DATABASE ASCII FILE 1.0
*PART* ITEMS
U1 7400
U2 7404
*NET*
*SIG* +5V
U1.14 U2.14
*SIG* GND
U1.7 U2.7
*SIG* mysig
U1.3 U2.1
*END* OF ASCII INPUT FILE
You may convert the .DCM file into a EDIF netlist with:
EDIF
EDIF is a standard for netlist format, see https://en.wikipedia.org/wiki/EDIF
The netlist looks like this:
(edif top
(edifversion 2 0 0)
(ediflevel 0)
(keywordmap (keywordlevel 0))
(status
(written
(timeStamp 19121 4 11 15 1 27)
(author "Data I/O Corporation")
(program "DASH to EDIF Netlist Writer" (Version "1.01"))
)
)
(comment " DRAWING DWG NO. DWG REF NOs.")
(comment "\TRYNET\TOP.DWG 1 1")
(comment "\TRYNET\SOURCE.DWG 2 2")
(comment "\TRYNET\DEST.DWG 3 3")
(library FutureNet_Primitives
(ediflevel 0)
(technology
(numberDefinition)
)
(cell &7400
(cellType generic)
(view PART
(viewtype netlist)
(interface
(port &1
(direction INPUT)
)
(port &2
(direction INPUT)
)
(port &3
(direction OUTPUT)
)
(port &7
(direction INPUT)
)
(port &14
(direction INPUT)
)
)
)
)
(cell &7404
(cellType generic)
(view PART
(viewtype netlist)
(interface
(port &1
(direction INPUT)
)
(port &2
(direction OUTPUT)
)
(port &7
(direction INPUT)
)
(port &14
(direction INPUT)
)
)
)
)
(cell top
(cellType generic)
(view DESIGN
(viewtype netlist)
(interface
)
(contents
(instance U1_1_2
(viewRef PART
(cellRef &7400)
)
(designator "U1")
(property PART
(string "7400")
)
)
(instance U2_1_3
(viewRef PART
(cellRef &7404)
)
(designator "U2")
(property PART
(string "7404")
)
)
(net mysig_1
(joined
(portRef &3 (instanceRef U1_1_2))
(portRef &1 (instanceRef U2_1_3))
)
)
(net (rename P5V_2 "+5V_2")
(joined
(portRef &14 (instanceRef U1_1_2))
(portRef &14 (instanceRef U2_1_3))
)
)
(net GND_2
(joined
(portRef &7 (instanceRef U1_1_2))
(portRef &7 (instanceRef U2_1_3))
)
)
)
)
)
)
(design top
(cellRef top
(libraryRef FutureNet_Primitives)
)
)
)
I see them named like this; QB<7:0>
Bus breakout wires are labeled 0, 1, 2, etc. as SIGs.
In this example, there are two busses. Even though the component signals are labeled the same (0, 1, 2 and 3), they end up on different nets.
The netlist ends up like this:
(SIG,,+5V,,,
PIN,1-1,1,U1,101,16
PIN,1-1,3,U2,101,16
)
(SIG,,GND,,,
PIN,1-1,1,U1,100,8
PIN,1-1,3,U2,100,8
)
(SIG,b,0,1,5,0
PIN,1-1,1,U1,21,15
PIN,1-1,3,U2,23,15
)
(SIG,b,1,1,5,1
PIN,1-1,1,U1,21,14
PIN,1-1,3,U2,23,1
)
(SIG,b,2,1,5,2
PIN,1-1,1,U1,21,13
PIN,1-1,3,U2,23,2
)
(SIG,b,3,1,5,3
PIN,1-1,1,U1,21,12
PIN,1-1,3,U2,23,3
)
(SIG,x,0,1,5,0
PIN,1-1,1,U1,21,11
PIN,1-1,3,U2,23,4
)
(SIG,x,1,1,5,1
PIN,1-1,1,U1,21,10
PIN,1-1,3,U2,23,5
)
(SIG,x,2,1,5,2
PIN,1-1,1,U1,21,9
PIN,1-1,3,U2,23,6
)
(SIG,x,3,1,5,3
PIN,1-1,1,U1,21,7
PIN,1-1,3,U2,23,7
)
But there are more questions... how do you connect a subset of one bus to another bus? What happens when there are multiple signal names on wires that are part of busses?
When I try something like this:
DCM.EXE complains "Multiple bus name on bus 'b'". Maybe this kind of thing can not be done.
I have not entirely figured this out. I know you choose an update library so that when new parts are defined, this is the library where they end up.
Also, there is a symbol edit mode. If you enter this mode after you have selected the 7404A inverter, it looks like this:
There are a bunch of commands for drawing various shapes that make up symbols.
I don't know how to add pins when you are in this mode. It does not seem to allow alphanumeric field entry when in symbol mode.
I think symbols end up being copied to the .DWG files that use them, because I can open a .DWG file without any libraries. This is different from OrCAD where the symbols are always by-reference to a library file. In OrCAD, if you modify a symbol in a library, you will see the change in all schematics that use it. If symbols are copied, then how do you update all instances when you make a change in the library? I know Altium prompts you to optionally update symbol instances after modifying the original.
