Certainly the BOSS-3 through BOSS-6 did not. The CPU was the DEC LSI-11, and the OS *was* the control program -- all in ROM.
Hmm ... just out of curiosity -- does his documentation show what kind of serial port chip is used to implement the RS-232 interface? I know that the BOSS-3 through BOSS-6 used old UART chips (40-pin chips so fairly easy to identify) and the only thing necessary with those to use hardware flow control would be to connect the proper pin through a RS-232 level translator chip (e.g. the MC1488/MC1489 pair (I forget which is the transmitter and which is the receiver, though I could always look it up) to the CTS pin of the RS-232 connector. IIRC, when there was data in the chip which had not yet been read, it would turn off the CTS pin to stop the flow without CPU involvement.
However, since form an earlier comment about it being run by a Motroloa 68000 family CPU chip, it is likely that it is using the MC6850 serial port chip (ACIA -- Asynchronous Communications Interface Adaptor) which required software configuration to honor/manipulate the CTS/RTS pins.
Does the system have a punched tape reader? If so, it should be able to stop and start *that* for drip feed, so what you need is an interface box to make that look like a serial port to the PC.
That sounds reasonable -- if the system sends a XOFF when it reaches the end of a line, and an XON when that line has been digested, that could work.
Hmm ... with a 68000 family CPU -- it theoretically *could* handle a *lot* of memory (for the time and the task -- up to 16 MB. (unless is a MC68008, which is limited to an 8-bit wide bus and to a 1 MB address space, IIRC.)
Yes -- analyzing it will give you more tools, at least.
"DoN. Nichols" fired this volley in news: snipped-for-privacy@Katana.d-and-d.com:
That's always been an easy one for me to remember.
"8" is binary 0x100. "9" is binary 0x101. The "8" value (1488) has an "O" at the end; "O" for "Out". The "9" (1489) has an "I" at the end... "I" for "In".
Gunner Asch fired this volley in news: snipped-for-privacy@4ax.com:
I've tried a lot, but so far there's not a lot of continuity to my trouble-shooting, for lack of time. "Ordinary" machining goes fine. It's just these long-trajectory engraving curves giving me fits, and I'll soon (after Jan 15th), get some real "sit down" time with the machine to figure it out.
ON the subject of modifying the boards to accommodate hardware flow- control: Why? If I'm going to start chopping things up, I'll just chop it ALL out and retro-fit. I have the tools now to do drip-feed, and wouldn't revert to a BTR, even if I had one. I was never keen on punched tape, even when it was the fallback medium of choice. One of the first things I ever did in the field was build a cassette tape system to replace the paper IPL tapes for our Data General Nova 1200's on my first "real" computer job.
My iron is in good shape, and a modern control would make this servo- based system a great platform. In the meanwhile, it does nice work if I just ignore (or work around) the ideosyncracies.
I have a potential customer coming on line that - if I win the contract - will permit me the income and time to retro-fit. I'll do it, in that case.
Mach3, i.e. "Mach3 3 axis servo retrofit package for Bridgeport type mills". With EMC2 there are various compatible modules available, but few if any turnkey kits packaged with all the components for a common retrofit.
What this means is that if you want to use EMC2 you have to do more planning up front to determine the set of "modules" you'll need for the conversion. You need to select interface cards, power supplies, servo drives, servo motors, encoders, limit switches, etc. as appropriate for the machine.
After the upfront planning, I don't think the time to perform the actual retrofit and get up and running would be much different between the two since you're doing the same physical work installing and wiring the components.
Thanks! *That* one I can remember. (Now the question is how many more times will I need to work with them? :-) I do still have some on hand for repairs or hardware experimentation.
How large an angle is that swinging? I know that some machines have G02 and G03 codes limited to 90 degrees swing at a time -- all in a single quadrant. If you cross over a quadrant line, you'll need two consecutive G02 or G03 instructions. Or three or four, depending on how many quadrants you want to cut in.
I don't know what the limitations of the BOSS-9 were.
"DoN. Nichols" fired this volley in news: snipped-for-privacy@Katana.d-and-d.com:
Through the BOSS-6, all the G2/3 instructions were single quadrant. G75/etc was reserved for multi-quadrant work.
However, although the BOSS9 has the G75 for backwards compatibility, it can do _almost_ a 360-degree curve with G2/G3. It does, however, use absolute arc centers, rather than incremental. I'm not even sure how to make it honor incremental centers, although it _must_ if it's to be compatible with the earlier BOSS controls. (It actually might be a board jumper I haven't identified yet.)
I have a Bridgeport R2E3 with Boss 8 control, with great success I have used Cadem NCNet Lite to flow programs to the machine under 12000 characters but have hit the limit when I started to use Mastercam (they like to do things the long way ). I have Ezlink and cable to port b , but from here I have not had results, I believe it may be a small error I'm not doing (such as the "-" when loading in REM, that took me a month to solve). Could you run thru the process from start to finish, what buttons you push, files you name ,program numbers etc you use. If it is easier , you can give me a phone number and I could call you or skype. Any assistance to get me past this hurdle would be very appreciated.
JB fired this volley in news:7decee28-60ba-4ce4-85b2- snipped-for-privacy@g26g2000vbi.googlegroups.com:
John, I sent you a long and detailed message yesterday on CNCzone, which I failed to CC to myself.
IF you got it, please forward it back to me so that I may re-post it here. Otherwise, I will re-compile it (which took a bit to get all the details right), and I'll stop using CNCZone for PMs which seem to get lost.
JB fired this volley in news:7decee28-60ba-4ce4-85b2- snipped-for-privacy@g26g2000vbi.googlegroups.com:
Here it is, John. I hope this turns the trick.
-------------------------------------------------
Drip-Feeding a BOSS-8,9 Bridgeport Mill.
First of all, my machine is a BOSS-9 R2E4, so there may be differences between how mine and an R2E3 BOSS-8 machine works. However, I have an operator's manual for the Series I R2E3 with the BOSS-8, and except for some display differences, it seems pretty much the same.
I have successfully drip-fed programs as large as several hundred K worth of g-code without error on my machine. My configuration is:
-BOSS-9 R2E4 (ca. 1986)
-Dell Laptop (Precision M4300) running Windows XP with a _hardware_ RS232 port (this may be important, I have not used a USB "dongle" to experiment with, yet.
-Original (DOS) Bridgeport EZLink software. There is no version reported. I've even looked it over in a hex editor, and the only date- specific thing I've found is that it was assembled around a 1987 version of the Microsoft run-time libraries. The specific file to use is "LDEZLINK.EXE".
(some of the following is not "drip-feed specific", but worth reviewing.
-I use a g-code file produce by CAMBAM (pretty much any CAM software will work, I guess, but CAMBAM suits my needs, and has a post-processor that is adaptable to make the R2E4 behave. I was using G-Simple, but there simply is no comparison in how easy or well it works.
Points about the g-code:
1) no matter what else, the DNC files must have line-end terminations of LF/CR, which is exactly backwards from what ordinary text files have (CR/LF) and also opposite what you can upload to the machine for a "remote load" program (don't ask why). If your post-processor doesn't allow you to specify the line-end sequence, you'll have to edit the file with a hex editor like XVI32 in order to alter what your CAM system gives into the LF/CR sequence. I can't coach you on the specifics, because without a sense of what hex codes are and how they look when editing a raw hex file you're going to have to develop some skills. You may already have them, though.
2) the BOSS9 _hates_ the G98 code; dunno why, because it ignores other invalid codes. Delete them entirely from your g-code.
3) the BOSS9 wants G2/G3 codes to be "center absolute" when in G90 (absolute) mode. I have not used it in G91 (relative) mode; don't intend to.
4) the BOSS9 expects ALL drilling and peck target depth and peck increments to be UNSIGNED distances relative to the stock surface. Negative values have weird results, even though -Z is the direction in which you drill.
5) a file destined for drip-feeding must begin with the "%" character alone on the first line, and end with a "%" alone on the last line.
OK... you have all the parts together, and you have a g-code file longer than 12K you'd like to upload. Remember that drip-feeding will give unexpected results on files short enough to fit in memory.
I have 10-meter RS232 cables, and have no problems with 4800 baud. If you have any lack of reliability, you may want to drop everything to 2400 baud. It makes a little difference in overall machining speed.
Set the "B" port on the Bridgeport to 4800,8,1,No Parity, No flow control... same for your RS232 port on your computer. Do this on the computer with the hardware manager so that EZLink doesn't have to fool with the settings -- it doesn't do it properly. Remember that, unlike the "upload to remote", DNC handles flow control within the DNC protocol, so any flow control feature you add to the port will introduce stray, unwanted characters into the data stream.
OK... ready to DNC (Direct Numeric Control) a program on the mill:
Before doing anything else, open a DOS window with "Run" and "CMD". Change directories to the EZLink directory.
I find it easiest to put the EZLink directory in the C:\ (root directory), since it's easy to "CD" to. Also, you should save a copy of the g-code file in that directory under the name "mygcode.txt" (or any other name you choose, with the .txt filetype). Start up EZLink by entering "LDEZLINK" at the command line. You should see EZLink fire up, and present you with a bordered black screen with function key definitions at the top.
Select "F1" to enter the filename. Use the directory name in which you stored the g-code file, and for the filename, give it the name you saved under the .txt filetype. When presented with a selection of "remote Load" or "DNC Link"; select "DNC Link".
On the Mill:
1) reset, enable axis drives, and home the machine.
2) Using the Load/Clear/Edit "clear" function, clear the RUN buffer ("0") and the PROGRAM buffer ("1" then "0" for "all").
3) Press RESET PROGRAM, and the program display should show empty ("[EOT]")
4) select LOAD "1" for DNC. The display will report "Setup Load DNC:"
5) enter a "-" followed by "execute". This tells DNC that DNC will supply the program name IF the program contains one. If not, the program will not have a name (which is OK, since it's not stored).
6) the display should now read "Setup Loading:-" and should report "DNC Off"
7) press "execute" once more. The display should now show "Setup Loading:-" and "DNC Link"
now move to your PC
8) The display on EZLink should now say "Filename: c:\yourdir \yourgcode.txt" and "Mode = DNC-Link"
9) press the "F3" key. The display should report "ready". IF you have established an RS232 link with the Mill, it will shortly report "Working". This says it has established control via the DNC protocol, and is actively "talking" to the mill.
If EZLink doesn't report "working", you have a communications error or no connection at all with the mill. Go back and troubleshoot your settings and connections. If you are able to remote-load programs with the mill and an Xmodem program, then the only thing that should change is the port settings for the "B" port, which must be 4800(or2400)8,1,N,none.
10) when the screen shows "working", return to the mill
11) Nothing will have changed on the display. However, prior to establishing the connection, nothing on the keyboard will have any effect except the Load/Clear/Edit function, which will ABORT the link.
AFTER "working" has been reported, pressing the AUTO key should allow you to select whether you wish to execute the program in automatic or single-block mode. Set it as you wish.
12) Once the execution mode is set, you may press "start" to begin cutting air or metal as your sense of risk permits!
I hope this helps. I'm pretty sure there will be differences between my BOSS-9 and your 8.1, but maybe not many.
"Lloyd E. Sponenburgh" fired this volley in news:Xns9E62D8818E359lloydspmindspringcom@216.168.3.70:
Hmmmm! 'Makes it almost not worth the hour and a half to compile all that information!
Not a peep! Three days of repeated requests from him for the info, both here and on CNCZone... complied with on the first day. No response, none. I took some time out of my day -- enjoyable time, but time I could have been cutting metal.
An e-mail follow-up to him; his response... "I didn't get it." OK, I'll RE-do it, because (my fault) I didn't save it, thinking he got it. (because he DID read it... read-acknowleged). And I apologize for not making sure I used a reliable medium .
I spend another hour on the machine and computer making sure every detail is nailed down. Write it up...(save it this time). Post it here. Email that I have done it. Email is acknowleged (by RSVP again).
NADA! Not a freekin' peep.
It almost makes you want not to help (but I won't succumb; there are worthies out there.)
replying to Lloyd E. Sponenburgh, R. White wrote: Lloyd,
I have searched for weeks trying to find the info you posted above. Thank you. Thank you We have followed your directions to a "T", it seems we have a port config error.. I will let my IT guy figure that out. Now on to another question, Your instructions were crystal clear in so much of a way that a novice to this antique CNC could follow your directions.
Would you have the time to do the same for entering code into the machine, manually from the console. I can get one line in, but after that, I am failing miserably. If that info I need to tell me the keystroke sequence, is in the manual, I did not see it or recognize it for what it was.
I realize this is a long shot, and would completely understand you not answering, but info is so scarce for this machine.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.