Dyna Myte 4400 (or other model) owners/users

[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