EIA to Dynapath Delta 10 via rs232

[cadman268]

Hi Guys

 

I have a dynapath post tweaked perfectly for mastercam but I remember reading that the control would accept EIA g code. Well I tried to get a generic fanuc post to go, but all I kept getting was a format error fault. Has anyone got it to go, I would like to know how they did it.

 

Thanks

 

Cadman268

[Hardmill]

Don't have your answer off the top of my head, but have you done a search to see if maybe

its been covered.

 

PEACE

[cadman268]

Nothing in the search for this----

[M. Anderson]

Cadman268,

 

I have a Delta 20 control on a machine.

(20 is just a updated 10 - same thing)

 

It has been a few years back, but I did use the MPFANUC.PST (modified) with some sucess. If I can find it I will see what's what, in the morning, and let you know.

 

It was something with the line numbers or the start of the file character? or

 

Later,

 

Mark Anderson

[cadman268]

That would be great, I know even the name (test) or whatever I call it, looks like its japanese before I get the format error, so it must be early in the file when it errors out, like within the first couple of lines.

Seems like the whole program loads, then the format error comes up when its done and the name in the catalog is P00000000 with zero bytes.

 

Thanks for your help

[LNDCAD]

Are you downloading this file from a computer over the RS232 port on the machine? It sounds like you have a communication parameter problem. The fact that even the file name "TEST" shows up as garbage characters suggests that the communications between computer and the control is corrupt. EIA is an odd parity format whereas ASCII / ISO is an even parity format. Even if you set parity to none, the code is different. I would look at the communication parameters (probably need 8-data, odd parity, and then make sure the stop bits and baud rate match). You might need to check out the communications section in your manual to see if there is any information specific to sending/receiving EIA G-code files. HTH.

[HEAVY METAL]

One thing cadman that might be causing a problem is the dynapath control needs an event type (e)-"for eia" before very line of code ex. N0001(E)G0X0Y0 let me know if thay was the problem

 

Thanks Heavy

[cadman268]

WOw, that sounds like my problem, What would I be into to modify a post to do that, could I add it to the end of each line number??

[M. Anderson]

Cadman268,

 

HeavyMetal, is correct, you can use a "(E)" after the program number to enter a EIA block as a conversational event. You may even mix EIA and conversational events in the same program, just not in the same block of code.

 

From my Manual:

 

quote:

---

"Event type" is not recognized as part of srandard EIA format, and you do not need to complete any entery here. However, you may program an EIA block as a conversational event by entering "event type" (E) directly after the N sequence number. If you choose to enter "event type" (E), you must follow the programming rules for a conversatonal event as listed.

---

I am going to fax you some sheets, rather than typing all this in.

 

LOOK FOR A FAX IN THE NEXT LITTLE WHILE.

 

Later,

 

Mark Anderson

[HEAVY METAL]

Hey guys let me know how you made out. Were you able to download a program in the EIA/ISO format without the conversational event type.

[cadman268]

Thanks M Andersdon,

I got the fax and am going to try after this program is done.

Heavy Metal, looks as though my main problem was that I had multiple G codes on one line. There can only be one of each type of code on each line and no spaces.

Does anyone have a post to do this. I have one I modified for a system C and it is setup that way, but I also had to omit decimal points and a few other wierd things to get it to work, to try and change it might be a challenge---LOL

 

Thanks Guys

 

Cad

[HEAVY METAL]

I don't think it will be as hard as you think. What post did you say you were using. If you could e-mail me it I could take a look. I assume your talking about multiable g codes at start of file and tool cahnge and end of file

 

 

 

Thanks Heavy

[cadman268]

It used to be a version of mpmaster till I got hold of it----LOL----I had to eliminate all G00's and output a G01 F200 for all rapid moves, and chage H calls to D calls and output the D tool length call on each line except for cuttercomp lines, then I had to output the D call for diameter. I also had to call the feedrate on eveyline as well, cause when I change to the f200 for rapid, it would stay that way....LOL

and more

 

I will send you a copy to look at when I get a chance.

 

Thanks

[cadman268]

Stop The Press

 

Got It

 

My main problem is that the comment text MUST be all in capital letters, I had them in lower case and it would not go....

Other than that it will load a fanuc post as long as it has the letter E at the very end, nothing at the start.

It will even take muttiple codes per line on this one. It adds the (E) all by itself

 

Thanks for everyon's help

 

Cad

[HEAVY METAL]

Glad things worked out for ya

[M. Anderson]

Yea, the post I had was a standard Fanuc post off the CD, just had some very minor modifications.

 

Glad you got it working!

 

Later,

 

Mark Anderson

[M. Anderson]

Heavy,

 

If you want - I will fax you the same sheets I faxed to Cad?

 

Let me know a number - may take till Friday - I'm leaving soon.

 

Later,

 

Mark Anderson

[HEAVY METAL]

Thanks MIke but i"ve got a dynapath manual .This is where got the info I gather.