[mmedina]

I just recently got a Dyna Mechtronics dm4400, and am looking for others who have experience with this machine (or the other similar models, like the 2400, 4000 etc) so that we can compares notes and tips. I've learned that the main issue with these machines is that they do not accept standard G-code, but instead use their own "Dynalan" conversational programming language. I would like to know how others have overcome this. Does anyone have the Dynacom software that originally came with the machine?

I've heard that this machine can be converted to accept standard g-code by purchasing Ahha's hardware card for around $3600 - ouch. I've also read that Bobcad and Mastercam have posts for this specific machine. What's your opinion on the best ways (and approx. price points) to make this machine accept commands from a PC?

All advice appreciated, as I know that your time is precious.

Mario

[donj1]

You're right about not taking g-code without upgrading. We have dm2400 and dm2800. They're a hassle to program until you get the hang of it(although I guess that's true of all cnc's). Biggest problem I have with them is having no graphics.

[Professorwiz]

I just got my Dyna 4400 Wired up and ready to go. I am having a problem with the startup process though and haven't gotten too far. It's only taken me 6 months to get this far..

[WTFisCNC]

I have a DM2800 and need some massive help. The boss bought it on e-bay and it came with nothing besides the cutting tools. No software or manuals. We did spend the $40 on a new set of manuals but that is it. Now that we have some down time the boss wants me to get this thing purring and I have no clue as to where to start. Please help!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

[Professorwiz]

I've started a Yahoo group just for Dyna Mechtronics users at
http://groups.yahoo.com/group/Dyna_M...ics_Users/join
perhaps try there?
Russ

[rebuildit]

WTF, Do you get the programming manual for the 40 bucks? What are some of the problems you are haveing?

[WTFisCNC]

I have the manuals. Iwill try the group. Thanks.

[WTFisCNC]

Does anyone know what programing language the 2800 uses and where I can find a crash course on it?

[DavidJSwanson]

I've used a dyna 2200 that we have at school. Which from what i've heard is basically the same controller on a somewhat better machine.

Mainly used mastercam to create the code, and then download it via RS 232 with Hyperterminal. If you want help/instuctions on hooking it that up let me know. Otherwise, I would think programming at the machine would keep any typos out.

Anyway, here's a REALLY FAST crash course. Please note that these explanations are written out from memory, so i think they're right but i'm not responsible if they're wrong.

I've written an explanation of what the lines do, then listed the code after that, only the first one is a complete program, the others are just parts that i pulled out of programs.

Line 849 - Shows start of program, inches mode, prog. no. 20
Line 850 - Tool Dia. .125 in
Line 851 - Feed Rate on X and Y axes to 16 in/min
Line 852 - Feed Rate on Z axis to 5 in/min
Line 853 - Halts the program and prompts you to set up the axes (if that's not in the manual, let me know and i'll go into more explanation)
Line 854 - Turns on the spindle, note on the left side of the spindle there's a switch that if turned off will keep the spindle from starting, also there's a local/program switch on the left front of the yellow box that transfers control of the spindle to the program)
Line 855 - "GO Fast" (rapid traverse) to X = -.3125
Line 859 - GO to Z = -.3750 (at defined feedrate)
Line 864 and 865 - using only one GO command and specifying two axes will do linear interpolation on those two axes (note that on this example that the Y axis is already there so it isn't obvious, this was a move to drill a hole, and mastercam likes to specify points that we're already at quite often)
Line 873 - turns off the coolant that was mysteriously never turned on using the COOLANT ON command.
Line 874 - raises spindle above clearance plane
Line 875 - turns off spindle
Line 876 - shows where program ends and gets machine ready to run it again.

.....
849 START INS 20
850 TD = .125
851 FR XY = 16
852 FR Z = 5
853 SETUP >ZCXYU
854 SPINDLE ON
855 GOF X-.3125
856 GOF Y-1.1875
857 GOF Z.1000
858 FR XYZ = 4.1
859 GO Z- .3750
860 GOF Z.1000
861 GOF X-1.6250
862 GOF Y-.4297
863 FR XYZ = 4.1
864 GO Y- .4297
865 Z- .3750
866 GOF Z.1000
867 GOF X-1.6250
868 GOF Y-1.9453
869 FR XYZ = 4.1
870 GO Y- 1.9453
871 Z- .3750
872 GOF Z.1000
873 COOLANT OFF
874 Z>C
875 SPINDLE OFF
876 END NEWPART
.....

Next segment of code show how to implement a tool change.
program is running until line 354, which raises the z axis all the way up.
then turns off the spindle. HALT will pause the program, allowing time for a tool change, until the "next" button on the keypad, which will resume program execustion, in this case it will turn the spindle back on and start motion again
.....
352 Z- .3750
353 GOF Z.1000
354 Z>ZMAX
355 SPINDLE OFF
356 HALT
357 SPINDLE ON
358 GOF Z.2500
359 GOF X5.0938
.....

This next segment show how circular interpolation can be specified.
starting at line 14 a local zero is specified to be at at 0,0 on lines 15 and 16. Line 17 tells it to "Go Relative angle" 90 degree CCW motion. (negative values indicate CW), i believe values up to 360 degrees can be used and there is a special command that needs to be used when the center is outside the machining envelope (i think it's an "i" or something, but i've never used it so i can't say for sure). Line 18 executes the move.
.....
012 GO Z- .0938
013 FR XYZ = 12.0
014 ZERO AT
015 GO X .0000
016 Y .0000
017 GR a 90.
018 >REF COODS
.....

[donj1]

This is some good info. We have a new man starting to run the Dyna so I printed out your info and will give it to him.

[DavidJSwanson]

Glad to hear it's of some help

Do you actually have a language reference book? I know there are some other things like helical interpolation, and drilling/milling canned cycles that i can look up and post later if you don't.

I think it would be nice if you can post any issues that a new person has learning the machine, as there don't seem to be many resources online about these controllers.

[Professorwiz]

David and others,
I've moved the Yahoo group to a board I've setup at www.professorwiz.com (click on forums)
David it would be great if you would post your example there. I've started posting examples like that, actually I started with a small boss yours gives a very nice detailed explination that I didn't actually get to yet. Thanks again for the great example. I've got a 4400 and it's program is exactly the same.
Russ

[Kid1000]

I have a DynaMyte 4400 in my work and i use it daily.
But it´s timeconsuming to manually program it line for line.
Anyone have postprocessors?

If anyone needs help in programming, feel free to ask me and I´ll try to reply.
I use this machine daily from 2002.

[Caprirs]

I worked for Dyna for a few years as a service/application tech. By the time I started, those old SKIP (single key input programming) controllers were already gone and Dyna was phasing out the Mitsubishi Meldas controls. Unfortunately, the designer of the SKIP control (Sandy Walker) passed away unexpectedly and did not leave good documentation. I had limited knowledge of them except for a few service related issues. I never learned the programming code so I am of no help there.

The Dynacom software was a DOS program that was used for RS-232 file transfer. Any other program will work as well like Hyperterminal, Predator, or ProCom.

As far as I know, all the manuals and software are still available from Dyna. And I think the price is negotiable if you're willing to barter a bit.

Most people that liked the iron but hated the control switched to the Ah-Ha setup because there was no limit to the file size and it recognized conventional G/M codes. Although I never dealt with the conversion, several customers thought Dyna should have purchased it and offered it as a retro-fit. The idea was floated around internally as a way of reducing the phone time our techs spent with customers who bought used SKIP control machines.

I currently use a pair of Dyna DM4400M mills with the Mits controls which are more conventional and allow for rigid tapping and more complex programs.

[DavidJSwanson]

I've posted out of mastercam 9.1 before to a DYNA MYTE 2200. Only downside i had was the 900 line limit built into the controller (i'm assuming you have RS-232 set up to a PC).

I've heard there's a program to drip feed a program to the controller but i've never seen it in use.

This was in school and i should mention that some students had "weird things" happen with fairly simple programs. I'm not for sure if it was the post or not.

-David

[rr167]

I have a Dyna 2400 that I am in the process of converting to run off a PC. I started by purchasing CNC pro. I then made a circuit board to be able to run off of the original power supply and motors. That worked OK but the motors are a little weak and replacement parts are $$. I really like the metal this machine uses so I decided to try something else. I bought a Closed loop step motor kit from MaxNC.
I am very close to finishing up. I just need to make some brackets for the limit switches and I should be ready to go. I teach at a Tech school so I am having my students make most of the parts. And remake them very often. I will post my progress

[Professorwiz]

Check out the forum I made just for Dyna users! It's at www.professorwiz.com. There are a few other people who have done retro fits as well. There is a person on there that is having an issue with the limit switches.
Russ

[jetpig1]

Hi folks, I bought a Dynamyte 2400 and have been tinkering for about a year and a half. The controller presents problems like you can only run 999 lines and then you can feed more code to it to do 999 more. I believe this is paging. You can get software to "drip Feed" pages if you have larger programs, but that gets complicated. The EPROMS in my controller died with the sound of an angry mosquito, and so I faced replacement of the whole thing. I got a DeskCNC controller and software, replaced my stepper driver boards, and I can now do huge programs and complex surfacing. I also replaced the steppers with 276 oz/in ones from Automation Direct, that make the old 20 oz/in units a little silly. If you want to get real sick, replace the 1/2 hp spindle with a 3 hp Porter Cable router motor and you have a force to be reckoned with.... [email protected]

[justin_sane420]

Heres some post processors for mastercam version 9 and 10 including the 2400c control 4400c control and the lathe (d)y300 control as well as a generic v9 post for the dyna.

figured this would help. As long as you arent using cracked software. Trust me. Big time trouble.

[jetpig1]

How can you modify these posts ? They don't open in Wordpad, like many other posts. - Curious