DYNACOM.EXE WANTED!!!!!

[dammachines]

i dunno. anyway i posted a question on that video, maybe i'll get an answer that would help make a working post for bobcad or anything else for that matter. we could only hope that there is infact g code support in the machine like there is in the 3000h. the bobcad posts are pretty simple to edit for g-code output.

I wondered if the YouTube comment was related to this discussion that I had seen a few days prior. Sorry to have to share the bad news, but my 3000H in that video is no longer running the original Dyna control. It was retrofitted with an AhHa controller before I purchased it so it does run somewhat standard G Code.

So after reading your comments, I took another look through my Users manual. I see nothing to lead me to believe that the 3000H ever supported G Code. The only mention of G and M Codes that I see is Table 4.2 on pages 29 & 30 and that appears to just be a list of "the corresponding DYNA converstional words for many commonly used EIA coded words." It's just there so if you know G Code you could related it to the Dyna Language.

I did see recently that AutoDesk offered to create a Dyna post processor. Are you a paying subscriber? I have read recently that they're more apt to do such things for people with a current subscription. The Dyna language is quite different that G Code so I can see it taking some time to get everything working. I have the dynamyte.cps post open right now. I can try and see how difficult it would be to get basic functions working...

I do have the original controller here. I've thought about applying power to it before to see if it would come up. Have to look at the schematic and see which pins are the serial I/O. I wonder if dynacom would be able to send to it w/o a machine attached...

Dave

[danxj7x]

yeah, that was me. i also asked autodesk about the post processor. hopefully they will release one sometime soon. the thing you might have trouble with not having the machine attached is getting past the home procedure but maybe not. the machine lets you into manual mode to jog if you say no to "ready?" so it might go into the download mode.

i'm a fusion subscriber. not a paying one, but a licenced subscriber.

i've looked through the post processor for the dyna mill, and peeked at one for a fanuc lathe. it is hard for me to understand what is specific to the lathe and how to change it around. i may fiddle with it at some point, but i'm not a programmer. when you try to output a lathe toolpath with the dynamyte.cps post it returns an error that it doesn't support turning tool paths. the only thing i see in the lathe posts that's lathe specific is the spindle section. so it might not be too difficult to make it work.. it's just the fact that i don't understand everything i'm looking at in there that makes me feel like i'm wasting my time when i poke through it.

[dammachines]

I've done a fair bit of playing around with the post processors both for my lathe and just for the fun of figuring out other people's problems on the Fusion Forum (user damincin there.) And I'm a software engineer by day - though I've never done anything with java before.

If you add the line "capabilities = CAPABILITY_TURNING;" to the dynamyte post you'll be able to get it to generate code, I just tried it here. Now to compare this code to the manual and tweak it for a lathe.

I should have a little bit of time over the weekend to look at it.

Dave

[danxj7x]

I've done a fair bit of playing around with the post processors both for my lathe and just for the fun of figuring out other people's problems on the Fusion Forum (user damincin there.) And I'm a software engineer by day - though I've never done anything with java before.

If you add the line "capabilities = CAPABILITY_TURNING;" to the dynamyte post you'll be able to get it to generate code, I just tried it here. Now to compare this code to the manual and tweak it for a lathe.

I should have a little bit of time over the weekend to look at it.

Dave

Well that should more or less cover the point to point moves. The canned cycles will need some work. My brother is the programmer in the family. I may know some things but I'm no programmer and I'm especially not a network guy. It's good to have someone else on board who isn't as green with the fusion 360 post processors or coding. Thank you.

[dammachines]

So... do you know if the entire program has to be loaded to the controller before you can run it? Or are you able to feed more code to it as it runs? Just thinking that the canned cycles could be ignored and just let Fusion handle all of that. The only issue there is the programs can be a lot longer that way. There's work to be done for arcs, but the rest can be handled with just linear movements.

I may have already started working on this... Do you have the DM3000 programming manual? The code in the manual that I have is a bit different than what this post produces.

For instance, feeds are specified using F XYZ = xxx in this code, but my manual lists FR X/R = xxx (or FR X/M if using per min, not per rev). And my manual says coolant on/off is via "CONTROL 4" and "CONTROL 5" but this post creates "COOLANT ON" and "COOLANT OFF" commands (I've already fixed this on).

Hopefully my manual is current. : )

Dave

[dammachines]

Ok,

Here's my first try. I wouldn't trust it too much, but let me know what you think, and what the controller thinks about it if you're able to get that far.

Setting the "useSetup" property will get it to output the "SET UP>DCZX" line that my manual shows, but it's not well described what that does. I think it's for you to zero everything with tool 1, but I'm not sure.

I haven't done anything with the end of the file (onClose()) stuff, so that Z>C , TOOL 0 code might not be correct. Also haven't touched arcs yet.

Dave

[danxj7x]

So... do you know if the entire program has to be loaded to the controller before you can run it? Or are you able to feed more code to it as it runs? Just thinking that the canned cycles could be ignored and just let Fusion handle all of that. The only issue there is the programs can be a lot longer that way. There's work to be done for arcs, but the rest can be handled with just linear movements.

I may have already started working on this... Do you have the DM3000 programming manual? The code in the manual that I have is a bit different than what this post produces.

For instance, feeds are specified using F XYZ = xxx in this code, but my manual lists FR X/R = xxx (or FR X/M if using per min, not per rev). And my manual says coolant on/off is via "CONTROL 4" and "CONTROL 5" but this post creates "COOLANT ON" and "COOLANT OFF" commands (I've already fixed this on).

Hopefully my manual is current. : )

Dave

it's supposed to be capable of a line feed mode that feeds only as much of the program as it needs to run such as a sub program or canned cycle or macro but the normal moves will feed line by line. there isn't much documentation on it but yes it is supposed to run long programs over rs232. i haven't really tested it.

[Big Chips]

Dave.... i want to thank you for your help and comments...we all apreciate it very much

[dammachines]

Dave.... i want to thank you for your help and comments...we all apreciate it very much

No problem. I know what it's like to have a tool and want to use it... And I'm sure you don't want to tear that nice looking lathe apart if you can avoid it.

I'm having fun playing with this so far...

I was able to trace the signals from the connector on the power distribution board to the controller last night. Attached 5v & Gnd on the appropriate pins and I got this thing to come up! I've had this lathe since 2006 so it's been at least 10 years since this thing was on and it still has the last program on it that the previous owner must have run. Looks like it matches the documentation that i have - and hopefully the 3000 uses the same syntax.

Here's a slightly updated post to try. I changed the ending code, and I think I have the ARC 1 command correct. Give it a shot with Fusion when you get a chance.

Dave

[dammachines]

it's supposed to be capable of a line feed mode that feeds only as much of the program as it needs to run such as a sub program or canned cycle or macro but the normal moves will feed line by line. there isn't much documentation on it but yes it is supposed to run long programs over rs232. i haven't really tested it.

Yeah, I looked at the wiring diagram and it looks like the CTS/RTS lines are connected from the lathe to the PC so it should be able to flow control. I don't see those signals going into the control box itself, but not all of the lines have names next to them.

[danxj7x]

yeah it look like purely hardware flow control. the dynacom program looks like nothing but a simple dnc file sender. after seeing it run i don't think it's needed. edytornc can be configured to send the needed end of file signal which for some reason is hex value 1A or "substitute." the thing i don't get, it errors if the lines numbers are not sequencial and it only numbers lines 000-999 so although it claims it can run unlimited line counts over serial. this seems odd to me unless following line 999 with 000 or 001 is accepted as sequencial. and i don't get how you could run macros like that. how could a goto line command work if it can't hold the whole program in memory? i think they fail to qualify some of the limitations when they list the features. i have a feeling by "unlimited line count" they really mean you can run a program over dnc even if the memory is full, i still have a feeling you will be limited to 999 lines, and i think any sub programs would be limited to the available memory. i could be wrong, i guess the machine control could have some commands that dynacom listens for but there is no interface to put dynacom into any special mode for line execute.

i really don't plan to do anything complicated that i have to worry about that. i think edytornc will be my goto communication program and my programs should be under 999 lines, and maybe i'll get preditor to work too since other people already have it. i looks like it has the feature to add ascii characters into the end of the file transfer but i have to look up how it should be typed in so it sends the hex value 1a not literally the characters 1 and A.

[danxj7x]

Yeah, I looked at the wiring diagram and it looks like the CTS/RTS lines are connected from the lathe to the PC so it should be able to flow control. I don't see those signals going into the control box itself, but not all of the lines have names next to them.

they do go to the control box one way or another. all the wires in the cable are connected. i took out my db5 connector on my machine trying to diagnose a connection problem and all 5 wires that are used in the cable are connected in the machine.

[danxj7x]

dave i have to thank you for your work. it's a big head start. but there are some bugs and my manuals are awful. there is an illegal feedrate command on radius moves. i think i fixed that. the SET UP>DCZX is like a g54, some fanuc lathes use "work shift" instead which is only a z offset from the g28 "home" reference point but practices vary. some people just the tool offsets from home and leave any other program zero zeroed. it's not 100% necessary on most machines. on these machines it might be. the milling radius move probably would have worked with a slight edit but the arc 1 01 should work as well but it's more intended as a roughing canned cycle. i'm leaving it for now since it does no harm except for using an additional line. i'm not completely understanding the feedrate sections though. it's not outputting the value, it's only outputting 0 or 100. it's too late for me to research this. i may work on that tomorrow.

[dammachines]

Yeah, I expected there to still be plenty of issues with it right now. I ran one of my sample parts through the post, but since I didn't change the feedrate throughout the three or four ops I didn't see that "F XYZ" line come up. There's probably more in there waiting to be found. : )

So I understand the change you made there, but not sure why you pulled out the Z axis feed rate calls in onLinear( )? From everything I see you need to specify a separate feed rate for X & Z. Otherwise it will use the default (50mm/min I think). I'll take another look at the feedrate code that I put in there. My crappy controller doesn't let me specify feeds in IPR, only IPM so that's what I have set right now. Let me swap over to IPR and see what I get here. According to the manual, "There are four kinds of FEED RATES: (A) INCH/REV range 4 digits Unit = 0.001 Inch, (B) MM/REV range 4 digits Unit = 0.01 MM, (C) INCH/MIN range 4 digits Unit = 0.1 Inch, (D) MM/MIN range 4 digits Unit = 1MM.

Regarding the ARC, I can't really see an easy way of you making the "ARC 1 F n" canned cycle work with Fusion. I don't think there's an option in there to support canned cycles for arcs? Fusion is going to handle the roughing and finishing for you by outputting individual arcs for each pass. So we need to force n to be 01 as that value is the number of passes to take -- looks like you've changed the post to put the feedrate in there instead. According to the manual, if you specify the "F" parameter then it will leave material for a finish pass and that amount needs to be specified with an additional line of "FIN= xxxx"

Ok... just found the feed problem, the feedFormat was setup to not take decimal places for mm and only 1 for inch. Try changing to this:

var feedFormat = new Format({decimalsunit == MM ? 3 : 4), forceDecimal:true, trim:false});


Dave

[danxj7x]

Yeah, I expected there to still be plenty of issues with it right now. I ran one of my sample parts through the post, but since I didn't change the feedrate throughout the three or four ops I didn't see that "F XYZ" line come up. There's probably more in there waiting to be found. : )

So I understand the change you made there, but not sure why you pulled out the Z axis feed rate calls in onLinear( )? From everything I see you need to specify a separate feed rate for X & Z. Otherwise it will use the default (50mm/min I think). I'll take another look at the feedrate code that I put in there. My crappy controller doesn't let me specify feeds in IPR, only IPM so that's what I have set right now. Let me swap over to IPR and see what I get here. According to the manual, "There are four kinds of FEED RATES: (A) INCH/REV range 4 digits Unit = 0.001 Inch, (B) MM/REV range 4 digits Unit = 0.01 MM, (C) INCH/MIN range 4 digits Unit = 0.1 Inch, (D) MM/MIN range 4 digits Unit = 1MM.

Regarding the ARC, I can't really see an easy way of you making the "ARC 1 F n" canned cycle work with Fusion. I don't think there's an option in there to support canned cycles for arcs? Fusion is going to handle the roughing and finishing for you by outputting individual arcs for each pass. So we need to force n to be 01 as that value is the number of passes to take -- looks like you've changed the post to put the feedrate in there instead. According to the manual, if you specify the "F" parameter then it will leave material for a finish pass and that amount needs to be specified with an additional line of "FIN= xxxx"

Ok... just found the feed problem, the feedFormat was setup to not take decimal places for mm and only 1 for inch. Try changing to this:

var feedFormat = new Format({decimalsunit == MM ? 3 : 4), forceDecimal:true, trim:false});


Dave

it was late so maybe i goofed but i thought i put both the z and x feed rate within the same line. my manual shows "FR X /M" and "FR Z/M" notice the space after x and 2 spaces before z? it doesn't explain how this works in much detail but my manual has several sample programs and some of them have feed rates written as "FR XZ/M" or "FR XZ/R" there are clear errors in the manual but i figured i'll at least try this to save a line. as far as adding the feed rate into the arc moves, well i haven't played with fusion much but since there was already that F XYZ line in there i thought it might have something to do with the way fusion operates. i debated simply commenting it out... thanks i'll try that feed format. i has a suspicion the "1:10" and "100:1000" had something to do with the number of digits and i saw other things in the program that said "3:4" but wanted to do some reading on that since i was basically guessing. i'll try that..

[Big Chips]

sorry guys i am not much help...all this post processor stuff is over my head.

but I thought I would let you know that Fusion 360 is have a Black Friday-Cyber Monday special...$25.00 for a year subscription for Fusion 360 basic. I have the link if you need it to purchase

[dammachines]

Just in case you were interested... The ? and : syntax is a short hand way of doing an If statement.
So this: "(unit == MM ? 100 : 1000)" is replaced with 100 if unit is set to MM or 1000 otherwise.

It uses the feedrate times 100 if the units are MM or the feedrate times 1000 if the units are set to inches since the feed per rev units are in .01 mm or .001 inches.

For feed per inch it uses times 1 or times 10 since the units are in 1mm or .1 inches.

No guarantee that I have this right though. : )

Dave

[danxj7x]

ok got ya. thanks again!

[danxj7x]

ok just realized the post i posted was the wrong one. i had realized that the "f" in the arc command was for finnish and had changed it back. i somehow uploaded the wrong file which i saved before i finished changing the feedrate to one line. just added the correct feedformat line

bigchips, if you haven't already built a cable you may be able to just get a "null modem" cable d sub 9 to d sub 25 it might work as is. i'm not sure if the jumper on the pc end has any importance, some old software doesn't support those pins at all so the pc may recognise that they aren't being used and use the rts ctr pins alone for flow control. you could also jump the #6 pin to the #20 pin in the machines connector to make that jumper so that you could use any null modem cable in the future. it seems like it's hard to find these cables with removable hoods these days but i found one on amazon. the ends and hoods alone are easy to find.

i think the post should work now but i haven't been out to the garage to test it. the things i see that are not consistent with the book are all a matter of spacing. it's not clear how important white space is in these programs. in most languages it's not all that important but it will be a easy fix if it is. this should be enough to get us turning parts. next step is to set up the threading cycle.

[dammachines]

I just noticed another section in the manual 10.5 Generating Arcs. Looks like there is another way to do an Arc which is more like a G02/G03 and doesn't use the canned cycle. And it only uses 3 lines so it will save some program space if that becomes important.

Fusion will already position to tool at the start point of the Arc before the call to onCircular. The only thing needed with in onCircular is

GO R (radius)
X end x position
Z end z position

The sign of radius determines the direction of the arc just like with the ARC 1 command.