Hiedenhain controls

[mayday]

after spending all week working on my post for a 310 control. I'm not imprest with hiedi's version of Gcode. Basicly my post works for conversational output quite well. What I'd like to know, has anyone managed to get the ISO version to work good?? the control seems to be very picky on everything including where spaces are. nothing like a fanuc. I've tried the ISO post but the Hied errors out on P values in the drilling cycles. not sure what it dosnt like.

[G Caputo]

Mayday,

 

This is from Dave Thomson from an earlier Heidenhain topic

quote:

---

Sounds like perhaps you are using the ISO code format, expecting it to be similar to standard G-Code. It's not. And the while it looks the same, the differences will drive everyone grey and bald, if not mad. For instance arcs use a two line format.

---

Just out of curiosity, if the conversational post works, why would you want to make the iso post work also? We tweeked in the conversational post to our specific machines and it works flawless. All of our Heidenhain controls are set up conversational and that is like a second language to me. To me making the machine iso when you are used to conversational would be like learning another control. Just curious on your reasoning.

 

Greg

[Claus@Cimco]

If you have a Heidenhain control you really don't want to run it in ISO mode. It's pretty much like running a Ferrari on 165/70 14 tires. Use the time it takes to get used to the Heidenhain programming language and get a real Heidenhain post.

 

 

Claus@cimco

 

[ 09-26-2003, 10:51 AM: Message edited by: Claus@Cimco ]

[mayday]

hied dosn't like helical ramp i.e x,y,z during arc moves in conversational, but it will do it in ISO

[Claus@Cimco]

you can do helical moves with a Heidenhain. You just have to use CP (polar) arc istead of CC arcs

 

Claus@cimco

[G Caputo]

Mayday,

Just made a 10" circle and helical milled it with a .5" pitch x 1" deep and this is what the mastercam code looked like from our post

 

5 ; 1-1/2" APFT

6 TOOL DEF 4

7 TOOL CALL 4 Z S1000

8 L W-4 R0 F MAX M3

9 ;

10 L X+0 Y+0 R0 F MAX

11 L Z+.1 R0 F MAX

12 L X+0 Y+0 Z+0 F120

13 CC X+1.9658 Y+.807

14 C X+3.9316 Y+1.6141 DR+ F160

15 CC X+0 Y+0

16 CP IPA+180 Z-.25 DR+

17 CC X+0 Y+0

18 CP IPA+180 Z-.5 DR+

19 CC X+0 Y+0

20 CP IPA+337.68 Z-.969 DR+

21 CC X+0 Y+0

22 C X-4.25 DR+

23 CC X+0 Y+0

24 C X+4.25 DR+

25 CC X+2.125 Y+0

26 C X+0 DR+

27 L Z+1 R0 F MAX

28 L Z+5 R0 F MAX

29 STOP

 

I myself have never helical ramped with mastercam, I like to approach the tools of the part whenever possible. Mastercam outputs only half the circle at a time where as the heidenhain control itself will do 5400 degrees of revolution with 1 circular move. ex: CP IPA+720 Z-1 DR+ RL F160. This is what the line would look like with no aprroach or depart to the centerline for a helical interpolation for a 1/2" pitch x 1" deep. I also don't know if the 310 is capable of this as we have 400 series controllers. This is just coming from a Heidenhain programmers standpoint, I'm still as green as they make 'em when it comes to MC.

 

HTH,

Greg

[mayday]

Thanks greg. I've gotta look at the post now that you showed me that. I am hard core fanuc output so this heid stuff is making my head hurt. why did they have to make there own so called gcode

[mayday]

just a note we did try that but on a deep helix say 5 or 10" it errored out because of to many degrees

[G Caputo]

Mayday,

I'm not the brightest when it comes to mastercam, but if you can send something simple to me of what you are trying to do, I will post it out and see what it looks like. I can then manually program it though with my eyes closed and tell you what the code should look like. All this gcode in here is like gibberish to me, except I am the minority with this Hedenhain stuff. So anyway I can help, feel free to ask.

 

Greg

[G Caputo]

Mayday,

What did you punch in and what was the error?

[mayday]

contour/ramp does work!

it just puts in a lot of arc moves do to the controls limit of degree revs it can handle.

thanks all

[Oppiz]

I use Heidenhain

ISO post everyday and it works great.

Post out... send it to the machine, no problem!

 

Its a TNC 370 control.

My post is a modified version of the default MC post hied_iso.