Heidenhain post processor tnc 426 chip breaking with pilot hole and gun drilling

[harunV2DKQ]

Hello,

I have a Mikron VCP 1000 TNC 426PB.

Post processor is basic from fusion 360

In the attached SS nc code, when I select chip breaking and gun drilling, an error appears = 17 cycl def, if I create new same cycle it in control it works but nc code is identical.
Second, I should arrange the post processor to use chip breaking with a lower RPM approach and feed into the pilot hole, after which the chip breaking cycle should begin.

how could you solve it?

Thanks in advance

@members @all

[harunV2DKQ]

[a.laasW8M6T]

Hi

The older controls don't support Cycle241 gun drilling

For Cycle 203

It is that you are getting Q208 = FMAX which I don't think the TNC426 supports we can replace this with Q208 = 30000(Or whatever your max feed is)

and the Q256 Dist for chip breaking that isn't supported by the TNC 426.

You can comment out the CYCLE DEF 241 in the post and if you have use expanded cycles turned on in post properties it will post Guided Deep Drilling out longhand code.

With the guided deep hole drilling cycle in Fusion

32 L Z+5 FMAX
33 L Z-34 F100
34 TOOL CALL Z S1870
35 L Z-120.0469 F187
36 TOOL CALL Z S200
37 L Z+5 F1000
38 L X+14 Y+0 FMAX
39 L Z-34 F100
40 TOOL CALL Z S1870
41 L Z-120.0469 F187
42 TOOL CALL Z S200
43 L Z+5 F1000
44 L X+0 Y+14 FMAX
45 L Z-34 F100
46 TOOL CALL Z S1870
47 L Z-120.0469 F187
48 TOOL CALL Z S200
49 L Z+5 F1000
50 L X-14 Y+0 FMAX
51 L Z-34 F100
52 TOOL CALL Z S1870
53 L Z-120.0469 F187
54 TOOL CALL Z S200
55 L Z+5 F1000
56 L Z+15 FMAX

Try the attached post

[harunV2DKQ]

Thank you for your answer.

When I run the program, at z -10 the spindle stops instead of raising the revolutions to 1000, without revolutions the feed continues

[harunV2DKQ]

also, it happens to me when I use two different programs with the same tool, the emulsion does not turn on in the second program.

[a.laasW8M6T]

Hi

The spindle stopping is a problem with the machine tool and how spindle speed changes have been implemented in the PLC, Unfortunately I don't think this is something we can fix in Fusion, unless your machine has a specific format required for spindle speed changes that is different to how it is implemented in a normal Heidenhain controller.

When you say two different programs for the coolant, do you mean two consecutive toolpaths with the same tool?

[harunV2DKQ]

As for changing spindle rotation, I will check in the book.

If two or more different programs are generated with the same end mill, switch off the emulsion when switching to another program.