Heidenhain iTnc-530 Control: Anyone using this one?

[mmetzinger]

We have a machine here with this control on it and we have a slight problem: We cannot cut a G02/G03 arc on it to save our lives! We end up having to break all arcs into point to point code. It is quite unbeleiveable but sad to say this is a reality. Is anyone else out in the great machining world using this controller and if so, how does your code look to cut arcs?!??! I am at my wits end with this boat anchor and need some help. It is on a Mikron machine that we got about 4 months ago and we have had nothing but problems with it since we got it.

 

When I program, I set in my parameters Comp type: Wear, Comp direction: Left.

 

I can cut a simple rectangle, arc on and off, roll around corners, no problem, and it will run on the machine. Now, add the reality of a part that is not a rectangle and it craps out. I can run the same part on our Bostomatics and it will run fine. (of course I used a different post)

 

HELP!!!!!!!!! (please don't make me fill the bay with this POS machine!!!)

[Allan Brown]

It's a good control. The multi-axis features for internal WCS tilting, datum tracking according to a kinematic model on the control, 5-Axis tool length comp, etc., etc. make these controls (and the earlier 430) a treat to develop posts for.

 

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.

 

I'd suggest you use the Conversational code format. If in doubt, ask the machine tool AE. Usually they'll admit that no one back in Europe (for DMG, Hermle, Mikron, etc.) will support the ISO format.

 

I have posts for both the Conversation and ISO formats. Have your reseller request them from me.

[G Caputo]

Woohoo, finally someone in here speaking my language! I believe are dealer got the conversational post that Dave Thomson just described, by the way, works great. We have 2 tnc430's, 2 tnc415's, and either 2 425's or 426's (not sure which from here). Been programming these on the floor for 14 years and they all program the same in conversational. Just a few "upgrades" from a machining standpoint that I see from a machinist's side. 3d rotation switch is kinda cool for setting jobs at angles too, also makes programming with a universal head on, very simple. We used the same post for all of our controls making minor changes for differences in each machine. here is as sample of the code creating a circle:

 

291 CC X+10.75 Y+0

292 L X+10.75 Y+0 R0 F MAX

293 L Z+Q68 R0 F MAX

294 L Y-1.06 RL F20

295 C Y-1.06 DR+ RL F50

296 L X+10.75 Y+0 R0 F MAX

 

In conversational you have 2 options the rnd (round) button or the c (circle) button. you must describe a circle center before the circle. These are the gray keys at the bottom of the keyboard.

 

The extension on the control will be a .h file. Any questions I can answer, I'd be glad to help.

 

Greg