DM3000...Retrofit or Get going with RS232 comm?????

okay guys...i think i need some help here and suggestions.

I have a all original and functional...everything works on it DM3000. It has the optional door opener,air chuck,regular chuck and tailstock tooling and good inserts also. Controller batt was replaced a year ago and Dyna updated the firmware ass well around 1.5 years ago.

I would rather get the RS232 port to connect and work with my computer and then just upload gcode cad post part file in a fanuc6t post in the controller and make chips.

I purchased this lathe 1 year ago and just now have had time to get back on it an learn to get this thing making parts...I dont think a retro fit is a good thing for this since everything does work. i also have the programming manual also.

SO i have several old computers with OS system from win 95 to win98... and have the rs232 connector.

I have all the parts to build my own RS232 cable as per the book schematic..so if ANYONE has got this thing to work and work good chime in...I have predator to use to upload the programs to the controller also

I need to know com settings and what cables pinouts you may have used and ect ect...

im currently working on this myself. the com settings are a little weird. i dont plan to give up but wasn't able to send a file today. according to the book that i got with the machine the end of transmission signal is the SUB character in ascii and that might not be possible to set in all dnc programs, i don't have predator cnc so i can't say. and there are some typos in the book as well for instance instead of showing the lines delimited but CR (carriage return) and LF (line feed) it shows CL LF on one line and CL RF on another which is basically computer gibberish, those things don't exist. but in the text below it says if must be delimited by ";" (semicolon) and CR. in a fanuc control using g-code the lines are delimited by a semicolon and known on the control as EOB (end of block) so it makes some sense but the inconsistency of the manual worries me a little.

the end of the manual has basic/Qbasic code for a simple send/recieve program to run in dos which i think will run through dosbox in windows or perhaps if it can be compiled to .exe it might run in the command prompt. there is also a program from dyna that might run in an x86/dos emulator like dosbox but i haven't acquired a copy of it yet.

I'll definitely be reporting back with my successes and failures. i'm still a little skeptical if it will use a fanuc 6t post processor for g code. there is no mention of anything other than dyna code in the manuals. perhaps its fanuc 6t communication settings but as i make progress those questions will be answered.

please post your results...another member pmed me and is going to send me a copy of the dyna program...i will send it to you when i get it also.

well i worked on compiling the basic code today. i used "freebasic" which doesn't require an emulator but i had errors. free basic isn't a dev environment just a compiler and the syntax could be different from the basic version the original code was intended for. i think i got it figured out but my knowledge of basic and programming in general is limited. the program finally compiled and it opens but im not near the machine and my laptop has no serial port. i intend to test it during this week and i'm also waiting on a copy of the dyna program as a backup plan. once i can verify i have working software then i can verify if the cable works and then i can get back to trying out modern dnc programs. will post the compiled .exe when i can verify it works.

thanks....from what i understand if you can get a gcode posted program into the dm3000 it will run it... the issue is a post and that is where my research found that the fanuc 6t is the post to use with your cad/cam software.


not many of us actually have a DM3000 in original and full working condition from what i understand now days....

that's what people are saying, and the ";" as a possible line delimiter in the manual might be a hint to that but i'm still skeptical. i did email DYNA on the subject and there reply was a little contradictory. first they stated out right that the dm3000 doesn't use g-code it uses a conversational code. then they said something about using a "post processor" to convert the g and m codes to a conversational language. then they say "now there is a Fanuc Postprocessor called Fanuc 6t (simplified)" but didn't give any kind of context on where to get it or how to use it. then they directed me to this web site.

now i believe most of the Dyna Mechtronics milling machines take g code as well as the dyna language but i'm not seeing people actually using g and m codes on the dm3000 in practice.

there are apparently post processors for bob cad and mastercam. but after the release of mastercam x9 it's harder and harder to find old versions of mastercam that might have such an old post processor packaged into it. i used to have mastercam 9 and a library of posts but after an unfortunate typo i ended up doing a complete bit by bit over write of the entire drive it was on. now when i search for mastercam 9 downloads i find x9 but i'm not about software piracy. i don't consider mastercam 9 piracy because for a time they had it up in the educational section of their own website.

bobcad expects payment for most of there posts. the dyna one is not on there website that i'm aware. but perhaps i can create a post that will work. the post processors for bobcad are more or less human readable and openable in a text editor.. it's just another project for another day.

bobcad is what i have and they told me to use fanuc6t post. I have a few friends that have mastercam 9 and I can call them to see what they have.

from my understanding...it will run a program that has been posted with gcode...but you cannot input gcode direct into the machine by hand...maybe that is where you are confused

update, i had some success today with rs232 communication. turns out my cable was bad. there was a manufacturing problem with one of the ends. so now i can get code to the machine with most dnc programs but it doesn't terminate the download mode at the end of the transmission. it gets stuck and all i can do is emergency stop the machine to reset the computer. i tried the basic program from the back of the manual i compiled but it doesn't work properly, it sends code but it errors the lathe out more frequently than the dnc software and it sends the code 1 character at a time forcing you to hold the enter key and i'm certain that's not how they intended it to work. im not sure it's worth fixing it, i just have to figure out the actual characters to tell the machine to end the connection and there might be some hints to that in the basic source code. i am currently using "edytornc" to send the files and it allows you to inject any code to end the program so once i figure out what i'm missing i'll be able to get it working from what i can see in the sorce code it might just be additional carriage return and line feed characters after the "sub" character.

now i did attempt to push code from bobcad with the fanuc 6t post processor to the machine. it failed to complete the transmission. so i checked to book for error codes where i learned the machine will not accept any line more than 16 characters including line numbers which take up 3 characters plus a space to distinguish them from code. so that leaves 12 characters per line. that can make things difficult to fit in g/m codes. if you need a dimension over a full inch with resolution down to a thousandth that's 5 characters, a space to separate it from the g command 2 characters for the g command leaving not enough room for another dimension. so even if it does work it won't even have the space in a line to make a taper because the x and z wont be on the same line, unless you maybe put the g1 on one line and the x and z on a second line. that may work with g1 but i don't think it would with radius moves. i just don't see it happening and wont spend any more time trying, even if it can run g code i'll have to edit all the lines down to 12 characters. it's just not worth it unless there is some situation where the line length restriction doesn't apply like maybe the line execute drip feed mode.

it also will fail if the line numbers aren't sequential. i'm pretty sure line numbers are necessary, really it's not looking good for the faunc 6t post. unless perhaps there is someone out there with a script or program to convert a g-code program into a dyna program.

i just received the dyna mech 3000h manual from fastest1 (thank you) and the 3000h does seem to take some g-code. perhaps if you have updated firmware yours may take g code as well but for my original 3000 it doesn't look good.

the com settings are 2400 baud, 8 data bits, 1 stop bit, hardware handshake, no xon/xoff. and as far as i can tell, if your dnc software enables you to, you want to inject a ascii character for substitute at the end of the program and maybe another carriage return and line feed. the ascii codes for these characters are 0x1a for sub, 0x0d for carriage return and 0x0a for new line or line feed.

my cable was made following the diagram in my manual but it shows db25 to db25 and no modern computers use db25 for serial, its usually parallel if it has a db25 and many dont have a parallel or db25 at all. i had to go by the pin functions rather than the pin numbers after searching for db9 and db25 rs232 pinouts. there are other diagrams out there that are essentially the same but with more jumpers. i can say on my machine those jumpers are un-needed as the machine doesn't actually have wires connected to those pins.

db9------------------------------------bd25

rxd 2----------------------------------------2 txd
txd 3----------------------------------------3 rxd
dtr 4-----|(jumper 4-6)
dsr 6-----|(on db9)
sg 5----------------------------------------7 sg
rts 7----------------------------------------5 cts
cts 8----------------------------------------4 rts

did he send you the dynacom software and if so have you set it up to use or try it

he thought he did, but it might have been on another drive. still waiting, still in communication with him. looks like auto desk has made a dyna post for the 2016 mill for hsm works, that should also work with fusion 360(free for atleast a year). now i have to see if it can be altered to work on the lathe. or if they will produce one for me. if you get g code to run let me know. i'm gonna hold off on trying that for a while.

I have sent it out a few times over the years. I am surprised someone hasnt chimed in with a copy. I have crashed and lost a few hard drives over the years with that file. Somehow it appears to have been lost. Still digging. Sorry. However I do have all of the other files for the 3000, 3000H, and 2400 models.

386 and early 486 computers are scarce and retrofits offer so much so i don't think too many people are using the dynacom program even if they have it. but i'm familiar with emulators and virtual machines so i think it's viable on a modern computer. these old machines were well designed. they did a lot with the limited resources. many of the mid 80's cnc machines did. i mean for such a simple machine it qualifies it's own backlash on startup. name a retrofit setup that does that!.. well i don't know if anyone can get in touch with tbirdgreg or who may have received the file but i hope someone chimes in. i promise that if i get the program i'll get it to run on a modern computer.

autodesk can make a post processor but i have to get them the scans of the manual. the machine and manuals are in my friend's garage so i can't photo them right now. fastest1, if you have another copy of the 3000 or 3000h manual would you please send it? the 3000h manual you sent is fine for the first half but the first file ends at about page 50 and the part 2 file is completely empty. the 3000h manual is much better than the copy of the dm 3000 manual that i have.

yes please send me the 3000H manual file also..it is alot better than the factory dm3000 manual i have

You both should have received every Dyna file I have. 3000, 3000H and the 2400. I did resend it all. Still no exe file though.