[FrankCNC]

Hi All,
I'm running a Heidenhain TNC 415A on a Tos WHN13.8 CNC and I've made a macro program in Heidenhain Language so I can Helical mill, Drill, Peck Drill & Tap at inclined angles with a Right Angle Drive Head. Every thing works fine except for the tapping where the spindle still runs and the m/c dwells for about 3 seconds after the tap has reached its tapping depth and consequently the compensation chuck extracts beyond its limit stripping the thread or breaking the tap.

Below is the sub program code for the tapping, I've tried removing the dwell cycle and placed an M5 at the end of the tapping depth line but all to no avail the spindle still runs and the m/c still dwells.

Hope someone can see where I've made a mistake or enlighten me how to fix the problem.

Thanks in advance.

3537 LBL 206
3538 FN 1: Q99 = +Q99 + +10
3539 FN 2: Q96 = +Q52 - +10
3540 FN 7: Q60 = COS+Q59
3541 FN 3: Q97 = +Q60 * +Q99
3542 FN 3: Q64 = +Q60 * +Q96
3543 FN 6: Q60 = SIN+Q59
3544 FN 3: Q98 = +Q60 * +Q99
3545 FN 3: Q65 = +Q60 * +Q96
3546 ;
3547 ; FAST FEED TO START POINT
3548 L IX+Q97 IY+Q98 R0 F5000 M3
3549 ;
3550 ; TAPPING FEED TO TAP DEPTH
3551 L IX+Q64 IY+Q65 R0 FQ56
3552 CYCL DEF 9.0 DWELL TIME
3553 CYCL DEF 9.1 DWELL 0
3554 ;
3555 ; RETRACT TAP BACK TO START POINT
3556 L IX-Q64 IY-Q65 R0 M4
3557 FN 9: IF +10 EQU +10 GOTO LBL 210

[hansdie]

so the problem as I see it is that your spindle is not stopping fast enough at the bottom of the hole thus over running the floating holder.

So couple of things to do or change.
1. Make the spindle stop faster
2. In your code calculate how much further the spindle turns in 3 seconds of slow down and then compensate by having an M5 then another X,Y move line
ie
L IX+Q64 IY+Q65 R0 FQ56
M5
L IX+Q66 IY+Q67 R0 FQ56 ;slow down compensating line

but the problem with your macro is always going to be syncing the feedrate to the spindle speed in case some one changes the override. you can always read the values and compensate.

but what I would, try to, do is adjust the cycle 19 transformation parameters to reflect the right angle attachment. That way you could use Cycle 2 threading directly with all the power that comes with that cycle (ie synced feed and spindle and the ability to stop or estop in the middle of a tapped hole and the machine will recover by turning out of the hole automatiically.

[FrankCNC]

Hi Hansdie,
Thanks for your help, I'll try out your suggestions and post a reply on how it went, the tap is a 1/8 NPT so I have to be careful on how deep it taps.

Unfortunately Cycle 19 is unavailable on our m/c, it was only an option on the TNC 415B and later that's why I wrote the macro to be able to counter bore, drill & tap some deep grease holes at various angles on the component.

We have now also purchased a Universal Milling Head so I have to modify the macro to do some compound angle grease holes (X,Y & Z) on the component which should be quite interesting to see how it goes.

I'll check with Heidenhain Australia to see if an eprom upgrade option to a TNC 415B or later is available for our m/c.

[Jukka Honkanen]

Hi Frank

Check your parameters MP7120.0 - 2

MP7120.0 Dwell-time for change of direction of spindle
rotation in "tapping" cycle
MP7210.1 Advanced switch time of spindle for "tapping" cycle
with coded output
MP 7120..2 Spindle run-on time after reaching total hole depth

All the values are in seconds.

Jukka

[FrankCNC]

Hi Jukka,
Thanks for your help, the parameters are.....
MP 7120.0 : 0.3
MP 7120.1 : 0
MP 7120.2 : 0

Can't see any thing wrong there, I'm beginning to suspect that it's a delayed "axis in position" signal as I've noticed the Tos WHN13 CNC with Heidenhain control sometimes dwells for no apparent reason while it decides what it has to do next.

Regards,
Frank.

[plankman]

I know this thread is a few months old, but here's something to try:
go into your machine parameters, and then set the following parameters:
paramater 7500 to 1 instead of 0.
parameter 7510 to %000001 instead of %000000
parameter 7511 to %00

Make sure you back up your parameter set onto your PC before changing.

These parameters need to be set as such above to tell the TNC that you have a head on the machine. Heidenhain does not preset these, as they have no way of knowing whether you have a manually or programmable head or tilting table on your machine - consequently it may appear that the tilting axis option is not installed. It is, it just needs to be tailored to the type of head you have.

I presume you have a simple manually adjustable head.

Once the tilting axes are enabled just write your program in a single axis, and the machine will do the rest.

As a starting point, write your program in G19 tool points x minus.
set up your head to point 45 degrees down and to the left.
set tilting axis C=45
dry run your drill/tap cycle and the machine should drill and tap down and to the left. Play with it, you'll get the hang of it!

[plankman]

One more thing... when you are operating with tilted axis (axes) the machine will be hesitant to respond quickly to the handwheel or manual control.

I had a macro program to drill oil holes at angles inside of big bores, and the macro program always paused a bit, although the same operation using tilted axis (axes) with OEM drilling cycle g82 never paused at all...I think its got to do with the look ahead in the control.

good luck (if you haven't already got it working)
Al.

[FrankCNC]

Hi Al,

Thanks for your help, unfortunately our TNC 415A does not have cycle 19 for tilting axis. cycle numbers in the m/c are 1 to 17 & 20 to 24.
I've sort of got around the problem by using a compensation tapping chuck with a clutch which I have backed off to clutch out very early, seems to be working fine at the moment.
It would be nice to get a look at the code for Heidenhain cycles so I can see how they program the spindle in the tapping cycle.

Regards,
Frank