Rigid Tapping Question

[RJS100]

I setup a test sample with Fusion 360 to experiment with rigid tapping holes for the 1st time.
The test sample has a number of holes that I intend to drill and tap using machining wax so I can tweak the mill's rigid tapping parameters to achieve the best possible tapped holes.

On the Design side, I modeled the holes to be 1/4 x 20 x 1/2 inch deep.
On the CAM side, I spotted the hole, drilled it .6" deep + the allowance for the "Drill tip through bottom". My idea was to drill the hole deeper than the modeled hole to allow a place for some chips to drop into.

The problem. When I attempted to program the tapping tool path, I initially entered the tapped hole depth of .5" since the tapped hole was modeled as 1/2" deep. When I tested this tool path, the tap just came down to the top of the part, reversed direction and finished the routine (It did nothing). I increased the programmed depth to .6 inches, .7 inches and finally .8 inches. Nothing changed until I set the depth to .8", then the machine tapped down to a depth of .8 inches and tapped the hole.

I don't understand what is happening. With all of the programmed depths, the Fusion simulations looked correct, and the depths looked correct on the CNC12 graphic display. But only when I programmed the depth of .8" did the tap go any lower than the top of the part. I did verify the tool length offset and all is well.

As I am still learning Fusion and G-code, I posted this question on the Fusion CAM website and got the following response:

This sounds like a machine/controller issue to me
If we post the code out at those increments it correctly goes to those depths in the G84

(Tapping M5)
N30 T12 M6
N35 S689 M3
N40 G17 G90 G94
N45 G54
N50 M7
N55 G0 X1.75 Y-3.
N60 G43 Z0.4 H12
N65 G0 Z0.2
N70 G98 G84 X1.75 Y-3. Z-0.5 R0.1 P3. F34.45
N75 G80
N80 Z0.4
(Tapping M5 4)
N85 G0 X1.75 Y-3.
N90 Z0.4
N95 Z0.2
N100 G84 X1.75 Y-3. Z-0.6 R0.1 P3. F34.45
N105 G80
N110 Z0.4
(Tapping M5 3)
N115 G0 X1.75 Y-3.
N120 Z0.4
N125 Z0.2
N130 G84 X1.75 Y-3. Z-0.7 R0.1 P3. F34.45
N135 G80
N140 Z0.4
(Tapping M5 2)
N145 G0 X1.75 Y-3.
N150 Z0.4
N155 Z0.2
N160 G84 X1.75 Y-3. Z-0.8 R0.1 P3. F34.45
N165 G80
N170 Z0.4
N175 M9


I cannot see any reason in the code why it would not work

I am using the "CENTROID Milling swissi-005" post. Is there something specific to Fusion & this post that I need to be aware of?

Here is the Fusion file: https://www.dropbox.com/scl/fi/6w1hsw1z ... ik4v2&dl=0

Best... Richard

[suntravel]

Is the CNC setup for rigid tapping ?

G84 will not need F Value but Q for the pitch

Code: Select all

M3 S500 F27 .78 ; start spindle CW, set up for 18 pitch tap
G84 X1 Y1 R.1 Z -.5 ; tap a 0.5 deep hole at X1 Y1
Y1 .5 ; ... and another one at X1 Y1.5
G80 ; cancel canned cycle
...
; Using Tool 15 Rigid Tap 632
G84 X0 .337 Y0 .925 Q0 .03125 Z -0.35 R0 .1 ; tap first hole
G84 X3 .312 Y0 .925 Q0 .03125 Z -0.35 R0 .1 ; tap second hole, must use Q
G80 ; cancel canned cycle
...
; Using Tool 22 Rigid Tap 440
G84 X1 .862 Y1 .627 Q0 .025 Z -0.19 R0 .1 ; tap first hole
G84 X2 .862 Y1 .627 Q0 .025 Z -0.19 R0 .1 ; tap second hole, must use Q
G84 X4 .262 Y1 .627 Q0 .025 Z -0.19 R0 .1 ; tap third hole, must use Q
G80 ; cancel canned cycle

IMHO fusion is not featuring a cycle for rigid tapping, use Intercon, or hand edit the fusion G-Code

Uwe

[suntravel]

Centroid Post in Fusion:

Code: Select all

case "right-tapping":
      if (!F) {
        F = tool.getTappingFeedrate();
      }
      writeBlock(
        gRetractModal.format(98), gAbsIncModal.format(90), gCycleModal.format(84),
        getCommonCycle(x, y, z, cycle.retract),
        feedOutput.format(F)
      );
      break;

It is not designed to put out the Q value from the pitch in the tool lib

If I have time, I will make a Rigid tapping version...

Uwe

[Muzzer]

I've generated rigid tapping from Fusion no problem. I'm away from my machine right now but could it be that you need to select "use canned cycles" or similar within Fusion CAM?

You shouldn't need to edit the PP to get this working. I'll see how I did this later when I get back....

[RJS100]

Thanks! I did not see an option for "use canned cycles" or similar, so I am curious as to what settings you are using. Thanks for your reply.

Richard

[suntravel]

Maybe rigid tapping works also with F, I never tried it out.

But the PP is definitely not using Q, it is also not defined to read the Pitch Parameter from the tool lib.

Uwe

[Muzzer]

Yes, I checked back through previous NC files generated in Fusion and no matter what settings you choose, it uses F, not Q. There's even a check box in the Fusion PP for "use feed per rev" but this still outputs G84 with F. My machine doesn't have spindle positioning, so I have a tension compression tapping head. True rigid tapping might be a little more critical, so perhaps I'm not in a good position to comment really.

To be fair, Centroid describes G84 thus: "performs right-hand tapping using a floating tap head".

In the interest of science, I tried the generic Fusion / Fanuc milling post and it outputs the same G84 with F, regardless of the check box status.

It seems that the only way to implement Q (feed per rev) in Centroid is using Intercon, as Uwe says. It requires spindle synchronisation using the encoder and careful setup looks pretty critical: https://www.centroidcnc.com/centroid_di ... meters.pdf

Having said that, almost all of the examples of G84 I could find use F and convert the thread pitch into that vertical feed based on the programmed spindle speed. If you manage to implement Q in a modified Fusion / Centroid post, I suspect it may be quite an unusual feature. It will presumably require the Centroid controller to activate spindle synchronisation, which may require input from the Centroid team.

Perhaps I'm lucky that I have been using a tension compression head all this time. The other option is thread milling, which achieves "synchronisation" in a quite different way.

[suntravel]

True Rigid Tapping works perfectly with Centroid, I am tapping M3 with 3000 rpm, tap in an ER Collet.

Modifying the PP for fusion should be no big deal, since it can readout the pitch from the Tool Lib.

Uwe

[RJS100]

Thanks again for getting back to me so quickly. A bit disappointing news. I am still learning both Fusion and G-code, so some of this is a bit over my head.

I too played with the "use feed per revolution" and it made no difference. Before attempting rigid tapping, I posed the question on the Fusion Formum as to what the "use feed per revolution" does. Here is the response I received:

Whether the FPR check box does anything depends on the postprocessor/controller. For tapping/drilling this has no effect, other than removing the G98 for some reason(centroid). You are using a Centroid Controller, correct?

Rigid Tapping needs to be setup in the Post processor if you want to specify the thread pitch as a Q word in the G84 cycle. It seems the standard centroid post is not configured for rigid tapping using a Q value. This isn't really a problem though, according to the centroid manual it will still rigid tap with an F value though (it will figure out the pitch from the RPM/Feed).

On some controllers/posts the use FPR checkbox will change the way a cycle outputs although this is primarily used for drilling cycles not tapping. On My Heidenhain controller FPR checkbox has no effect for tapping as it only accepts a pitch, and drilling only accepts FPM.

I am going to ask where in the Centroid manual it says that it will still rigid tap with an F value by figuring out the pitch from the RPM/Feed.

I think I will try to reach out to Swissi and see if he has any insight.

Richard

[suntravel]

Mill Manual:

Note: If rigid tapping is enabled, a Q may be used to set the thread lead or pitch. However, because Q is not modal in
the case of Rigid Tapping, you must specify Q on every line at which Rigid Tapping is to occur.

All examples are with Q

Uwe