Tapping on HMC at an angle w/90° head pt-to-pt
Likes:  0

# Thread: Tapping on HMC at an angle w/90° head pt-to-pt

1. Aluminum
Join Date
Dec 2012
Location
WI, USA
Posts
214
Post Thanks / Like
Likes (Given)
70
10

## Tapping on HMC at an angle w/90° head pt-to-pt

Hello,

I have a programming question on a Mazak HMC with an M-Plus control (vintage 1996, I believe). I need to tap a hole, moving in both the X & Y axes simultaneously while tapping. The only way I would know how to attempt this would be point-to-point programming, but I'm not sure this would be successful and I'm not exactly sure the best way to program with this approach, anyway.

In order to tap the hole, I am using a 90° head that also rotates and is set at 20° in what would be the C axis. To drill the hole, I am doing this:

...
G54.1P1X#632Y#633B264.250
G43Z0.0000
G1X#602Y#603F100.0
X#604Y#605F30.0M8
X#602Y#603F100.0M9
G0X#632Y#633
...

Using #602 & #603 as my starting positions and #604 & #605 as the ending positions. These are the results of simple calculations based on the distance the drill tip is from the c/l of the spindle so new programmed coordinates don't need to be edited at every tool change.

So, how would could I program this to successfully tap this hole? Something like?:

...
G0G20G90G95S600M3M38
G54.1P1X#632Y#633B264.250
G43Z0.0000
G1X#612Y#613F100.0
X#614Y#615F.0492
M5
S600M4G1X#612Y#613F.0492
G0X#632Y#633
...

I'm thinking there has to be a way to do this and I'm just drawing a blank for some reason today.

Any help to straighten me out would be greatly appreciated.

Regards,

Paul

2. Shouldn't you be able to use regular canned cycles with the proper plane selection? Been a long day but I am thinking a G18 should set your "z" in your Y direction. Then you should be able to do a g68 and rotate 20 degrees so you can just program it as a "linear" move.

3. Also, are you trying to rigid tap?? May have better luck if you try and use a thread mill if possible

4. Titanium
Join Date
Feb 2007
Location
Aberdeen, UK
Posts
3,502
Post Thanks / Like
Likes (Given)
1217
1308
In order to do what you want using a tapping cycle, your machine needs to support some form of arbitrary work plane / tool vector.

On our Hurcos (and Fanuc generally) this is G68.2. I don't know enough about Mazak to say one way or the other, hopefully someone else will chime in.

In order to do point to point you will need to have a compensating tap holder on the end of your angle head, or the ability to program the spindle as an axis and do an interpolated XYC move.

As the poster above me stated, it would be easier to threadmill using linear moves, unless you can program arbitrary work planes on your control.

5. Aluminum
Join Date
Dec 2012
Location
WI, USA
Posts
214
Post Thanks / Like
Likes (Given)
70
10
Thanks to all for the replies.

358Mustang, I hadn't thought about incorporating the coordinate system rotation mode, G68 ... that is a creative idea. However, the 20° angle is already positioned because the right angle head can also rotate about the Z-axis. Then, the machine needs to move linearly at that 20° angle. Drilling is no problem because I can program each move line-by-line. When tapping, how could I do this? I'm afraid I won't have the code properly placed, resulting in bad threads. If G18 (or G19) plane selection was activated, I don't believe employing the G68 would would accomplish what I'm after. Maybe the only concise way to do this is if the machine has the option of executing a tilted working plane command that can automatically generate a feature coordinate system that is normal to the tool direction, something like a G68.3 on a Fanuc 31i-B controller.

If this machine does not have this option (I doubt it does, nor do I know if that would provide the solution), why can't I just mimic what the machine does in a normal G84 cycle? How do I find the code for this in the machine? This tap would be in a solid holder, not a tension/compression type, so is there a way to simulate a G84 synchronous tapping command, verses non-synchronous, if programming point-to-point?

If I can't create the threads via tapping, then I will explore thread milling because that appears to be a viable option, however we have the tooling for tapping the hole, not thread milling ...

Thanks again for any help.

Regards,

Paul

6. Aluminum
Join Date
Dec 2012
Location
WI, USA
Posts
214
Post Thanks / Like
Likes (Given)
70
10
gregormarwick,

I skipped right over your post somehow, and it looks like you already summed-up what I just replied with!

Thanks for the reply!

Regards,

Paul

7. Diamond
Join Date
Dec 2008
Country
UNITED STATES
State/Province
New York
Posts
10,032
Post Thanks / Like
Likes (Given)
0
2609
when not using a tapping cycle and just using G1 the danger is feed and rpm not at 100%. most tapping cycles ignore override selection and tap as programmed.
.
just saying if you are on 80% feed your rpm to feed ratio will be off considerably. not saying somebody would deliberately do but forgetting you are not at 100% feed and rpm has happened to operators before.
.
some machines especially with gearbox backlash continue to turn when slide has stopped moving and you can often see tap screwing into part a extra amount. when tap comes out of hole can often see extension compression spring pull it back suddenly when free of the hole. sometimes this extra tap turning tap hits bottom of hole and breaks

8. Originally Posted by acncguy
Thanks to all for the replies.

358Mustang, I hadn't thought about incorporating the coordinate system rotation mode, G68 ... that is a creative idea. However, the 20° angle is already positioned because the right angle head can also rotate about the Z-axis. Then, the machine needs to move linearly at that 20° angle. Drilling is no problem because I can program each move line-by-line. When tapping, how could I do this? I'm afraid I won't have the code properly placed, resulting in bad threads. If G18 (or G19) plane selection was activated, I don't believe employing the G68 would would accomplish what I'm after. Maybe the only concise way to do this is if the machine has the option of executing a tilted working plane command that can automatically generate a feature coordinate system that is normal to the tool direction, something like a G68.3 on a Fanuc 31i-B controller.

If this machine does not have this option (I doubt it does, nor do I know if that would provide the solution), why can't I just mimic what the machine does in a normal G84 cycle? How do I find the code for this in the machine? This tap would be in a solid holder, not a tension/compression type, so is there a way to simulate a G84 synchronous tapping command, verses non-synchronous, if programming point-to-point?

If I can't create the threads via tapping, then I will explore thread milling because that appears to be a viable option, however we have the tooling for tapping the hole, not thread milling ...

Thanks again for any help.

Regards,

Paul
I understand your angle head is at a 20 degree angle. That is what the G68 would be for (I have run many Mazak HMC's of the same vintage and they all had g68). All you are doing with this is rotating the coordinate system so your "y" axis is "parallel" (or x, depending on how the angle head is pointing) with your angle head. So if you have the proper plane selection you should be able to just tap at that angle.

I am not aware of being able to do synchronous tapping without having the G84 command. I would be concerned with backlash in the angle head while trying to rigid tap. It may work, but it also may blow out the threads...

9. Aluminum
Join Date
Jan 2014
Country
UNITED STATES
State/Province
Oregon
Posts
196
Post Thanks / Like
Likes (Given)
35
95
358Mustang has it nailed. I have done this successfully, but only with G68 and a canned cycle. Your scenario is basically what that function is designed for.

Also worth noting that the gears on MOST right angle heads are directional, and they are not supposed to be used for rigid taping.

10. Aluminum
Join Date
Dec 2012
Location
WI, USA
Posts
214
Post Thanks / Like
Likes (Given)
70
10
358Mustang & boosted,

I would need to run this G68 in the 3D mode in order to run a canned cycle at this angle, correct? This machine does not have that option. Switching to G18 or G19 then using G68 2D would not work because the direction of the 90° head spindle axis wouldn't be perpendicular to the new plane due to the 20° the tap is rotated down in the C-axis.

I've never used the 3D G68 mode, so I didn't think about it when you mentioned using G68. I was thinking 2D.

DMF_Tom B,

Thanks for the reply. Yeah, I'm not going to try to tap this hole without using a canned cycle.

Regards,

Paul

11. I Shirley kan't hep on a Yamazaki at all, but if you kant rigid tap it, using a compression/retention holder should be no different that drill the hole in the firth place.
At least that would git it started ... straight. You could finish by hand if required. (if this is a bottom app)

I cannot even imagine the code required to mill that!

----------------------

Think Snow Eh!
Ox

12. Titanium
Join Date
Feb 2007
Location
Aberdeen, UK
Posts
3,502
Post Thanks / Like
Likes (Given)
1217
1308
Originally Posted by Ox
I cannot even imagine the code required to mill that!
I've actually just done this. I have an adjustable angle head on a 40 taper, and I have a job with a lot of double angle holes to drill. I only have one machine with a 40 taper and it's ancient, no coordinate transform functions whatsoever.

I wrote a program in C++ to generate the toolpaths. I will probably upload it here when it's in a state where it's usable for others, on the off chance that somebody else might ever have a use for it.

The process to generate helical toolpaths is really just define the tool axis as a unit vector, define the axis of the helix along that vector, generate the helix around that vector.

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•