Updating Interact 2 Post

[Mic6]

So my co-worker is finally taking the leap from 9 to X4. So far so good. We updated the post using the Update Post c-hook. All the milling paths have been fine, but when we go to a drilling op, it wont post a Tool Call, it will try to drill with the last tool being an endmill. We've tried force toolchange, but that didn't work. It's a Heidenhain TNC 2500. I'm thinking we may have to add a block or set something in the MD/CD. Any ideas? Thanks AGain!

[Bryan Johnson]

check for the following variable and set to 0.

 

rpd_typ_v7$ : 0

[Mic6]

What does this variable do?

[Jim Evans from CNC Software]

rpd_typ_v7 is a flag that is used to tell MP how to interpret the drilling NCI. There was a change to the NCI format for drilling and this variable was added to allow backward compatibility.

 

The update post utility will actually add and set this variable depending on what version you are updating from.

 

Follow Bryan's advise and set it to zero and you should be ok. If not then we will need to see your post so we can review the drilling section of it.

[Mic6]

That was it. Works great now. Thanks again

[Mic6]

Having another problem here. The variable discussed above is still set at zero. The problem is when the program is posted, it's outputting the drilling feedrates as a negative # as shown. Everything else shown as negative is correct.

code:

---

 0 BEGIN PGM 1 INCH

1 LBL 200

2 L Z+0.551 R0 F6298 M91

3 L X+0.0 Y+0.0 R0 F MAX M05

4 LBL 0

5 STOP M25

6 TOOL CALL 1 Z S800

7 L R F M03

8 L X+0 Y+0 R F MAX M

9 L X+.68 Y-.5 R F MAX M03

10 CYCL DEF 1.0 PECKING

11 CYCL DEF 1.1 SET UP -0.1

12 CYCL DEF 1.2 DEPTH -0.5857

13 CYCL DEF 1.3 PECKG -0.045

14 CYCL DEF 1.4 DWELL 0.

15 CYCL DEF 1.5 F-20 <----------------------------------

16 L Z0.1 R F MAX M

17 L Z0.1 R F MAX M9

18 L Z0.1 R F MAX M99

19 L X+4.33 R0 F MAX M99

20 L X+4.338 Y-4 R0 F MAX M99

21 L X+.68 R0 F MAX M99

22 CALL LBL 200 REP

23 STOP M25

24 TOOL CALL 2 Z S800

25 L R F M03

26 L X+1.42 Y-.92 R F MAX M

27 CYCL DEF 1.0 PECKING

28 CYCL DEF 1.1 SET UP -0.1

29 CYCL DEF 1.2 DEPTH -0.5804

30 CYCL DEF 1.3 PECKG -0.045

31 CYCL DEF 1.4 DWELL 0.

32 CYCL DEF 1.5 F-20 <------------------------------

33 L Z0.1 R F MAX M

34 L Z0.1 R F MAX M9

35 L Z0.1 R F MAX M99

36 L X+3.57 R0 F MAX M99

37 L Y-3.57 R0 F MAX M99

38 L X+1.42 R0 F MAX M99

---

[Mic6]

No Interact love out there?

[Guest CNC Apps Guy 1]

Nope!

[Acro Engineering]

I had the same problem with an older TNC 151 post, I think I changed the FR$ to FRPLUNGE$...

[Jim Evans from CNC Software]

F-20 is probably a F-2. -2 in the NCI means it is a rapid move and no feed is present. Look at your drilling code and change fr$ to fr_pos$ or frplunge$ as suggested above.

 

Depending on how old the post is it may need to be update some because the NCI layout for drilling changed back a few version and when using fr worked back then it doesn't now.