Heidenhain g-code help

[arkum]

I am used to programming fanuc controllers and I have been asked to help out a friend with a heidenhain controller.
Are there and differences in the g code i have to use?
Any other advise or help/links is greatly appreciated.
Thanks in advance

[MIKE JEFFERS]

hiedenhien uses m code not g. its basically similar and from a beginners point of view
a lot eisier to manually program. if your using a cam system (i use dolphin) use the
TNCnnn POST nnn being control number (tnc150/151 etc) these are fitted to interact
mills ,try heidenhein web site for more
m codes you need most are m3,4,5, spindle start cw- ccw- stop & m25 -spindle stop/z retract, cutter comp RR & RL right/left os.Rads are CC circle ctr CE circle end. cycl def button gives cann cycles.And thats about it the rest is simple co-ord programming.hope this helps
mike

[HuFlungDung]

Hmm, I didn't know that all my cnc's are bilingual

[xtaffy]

Hi,

You can change the machine/cnc control parameter to work in ISO/g-code

[Daninwyoming]

Heidenhain has the MOD key. Go there and cursor up till you find the plain language-or- ISO switch. Many g-codes are similar to fanuc and differ mainly when you get into the canned cycles.

[Mr_Carpyman]

There is no reason why you could not program a Heidenhain control in ISO.
G codes and M codes will work check webs site for Heidenhain control level for G code use. There are a few minor differences as to how Heidenhain language handles some info. All linear movements are defined with an L and X,Y & Z absolute or IX,IY & IZ for incremental, circles & rads are defined with CC for the centre start point (can be absolute X,Y or incremental IX, IY)
and C for the circular move X, Y, etc. the DR cna be a + or - this indicates the direction of the arc. Heidenhain use an number of its own coversational type macros for pocketing, helixcal, drilling & tapping cycles these are quite simple and self explanatory.

Any reasonable programmer should have no problem in using Heidehain.

The lin below will help it has a wealth of info.

http://www.heidenhain.de/gb0.htm

[Navigator]

Sorry,but I've worked with heidenhain more than two years and my opinion is that it's just waste of time to use this controller in ISO mode. It has very simple and powerfull conversational language (for milling applications) which makes programming much easier. I'm working with fanuc and heidenhain,every has it's own advantages and "black spots" but heidenhain excellent in it's conversational programming,once you understood it,will never forget,I swear I mean controllers series 355 and above..407,415... 426... worth to try...

[F.Sharifi]

Originally Posted by arkum I am used to programming fanuc controllers and I have been asked to help out a friend with a heidenhain controller. Are there and differences in the g code i have to use? Any other advise or help/links is greatly appreciated. Thanks in advance

Hi
you can change any Heidenhain controller system from TNC 151 up to iTNC 530 to programming with G cod or HeidenhainPlane Language . its depends on what kind of control system that you ask to know . for example for TNC 155 its just needs to change the Machine parametr . but in TNC 426 its easy ,...just choos program selection typ ISO or Heidenhain .

OK Iam expert on Heidenhain p[lease let me know what exactly you want !

Regards !
F.Sharifi

[yemoro]

Hi.

we are going to buy a cnc milling machine (kern) with a iTNC 530 control. We are currently using solidcam to writte cn programs and use cimmco software to transfer codes to our cnc leadwell 300 by serial port. We need to know if we can send directly cnc (iso) codes to iTNC530 control by this kind of serial port or we need to convert to heindenhain code. there is a better option you can tell us?

[xtaffy]

Hi,

In the parameters of the system you can change it over to G code

[CNCRim]

This is Heihen code look like:

0 BEGIN PGM 12345678 MM
1 L M09
2 L M05
3 TOOL CALL 03 Z S15000
4 L M06
5 L M03
6 L X-51,000 Y+4,748 R0 F9999
7 L Z-5,000
8 L Z-13,320 R0 M08
9 L Z-18,570 R0 F1500
10 L X-51,181 Y+4,472 R0 F3000
11 L X-51,341 Y+4,278 R0
12 L X-51,509 Y+4,115 R0
13 CR X-51,858 Y+3,875 R+1,774 DR- R0
14 CR X-52,259 Y+3,736 R+1,448 DR- R0
15 CR X-52,698 Y+3,728 R+1,315 DR- R0
16 CR X-53,232 Y+3,925 R+1,450 DR- R0
17 CR X-53,538 Y+4,157 R+1,859 DR- R0
18 CR X-54,000 Y+4,748 R+2,454 DR- R0
2005 CR X-68,438 Y+16,043 R+1,592 DR- R0
2245 L X-34,194 Y+15,929 R0
2246 CR X-34,177 Y+15,531 R+1,592 DR- R0
2247 CR X-34,264 Y+15,087 R+2,005 DR- R0
2248 L X-34,352 Y+14,851 R0
2249 L X-34,500 Y+14,557 R0
2250 L X-42,872 Y+0,055 R0
2251 L Z-5,000 R0 F9999
2252 L M09
2253 L M05
2254 STOP M30
2255 END PGM 12345678 MM

[F.Sharifi]

Dear Sir
in the iTNC 530 the connection for RS232C and RG45 ( LAN ) is standard , with Cimmco Edit you can translate any Heidenhain to G code file ( go NC Function then find in this column the HEIDENHAIN/ISO Converter ) ,...

in this control you have go in manual mode press MOD key then choose the program input with ENTER key you can choose Heidenhain or ISO or Heidenhain/ISO

last things based on control software version and machine MD you can have or have note somthing , please change your data transfer with LAN cable and use TNCRemo its very easy to use and safe ,..and you dont need to tarnslate any program because control can accept and run any G code or Heidenhain if there are in memeory

let me know if you have any trouble iam expert on heidenhain
F.Sharifi

Originally Posted by yemoro Hi. we are going to buy a cnc milling machine (kern) with a iTNC 530 control. We are currently using solidcam to writte cn programs and use cimmco software to transfer codes to our cnc leadwell 300 by serial port. We need to know if we can send directly cnc (iso) codes to iTNC530 control by this kind of serial port or we need to convert to heindenhain code. there is a better option you can tell us?