Path Feature #8018 - G84 Canned Tapping Cycle

[luvtofish]

I know this has been brought up before but wanted to see if any work has began on this front. Tapping on a CNC is every bit as crucial as the drilling cycles. Rigid tapping aside, just having the ability to perform a rudimentary G84 canned cycle with a required tap holder tool would close a huge functionality gap in Path.

I'm no programming expert, but would think this could be implemented in a similar fashion to the G81 drilling cycle. Needed functionality would include specifying tap size & spindle speed (to calculate feed rate), Z depth, R Plane, etc. The canned cycle would need to understand how to halt the spindle, dwell and reverse spindle on the retract. Easy Peasy right?

Would love to see priority given this highly needed enhancement. I'm sure I'm not the only one who feels this way.
I'm willing and available to assist to make this happen -- just need somebody who understands the Path internals better than I do.

Cheers!

Dan

[GeneFC]

G84 is intended for a TapMatic style tapping head. There is no spindle reversal, only a dwell time.

Your description is more akin to (but not the same as) rigid tapping, not G84.

Gene

[luvtofish]

This is not true for my Control and I'm sure others as well. Rigid tapping on the Dynapath Delta 40 to 60 is called out with a G75. G84 performs exactly like I mentioned above. I currently have to modify the code manually to tap holes on this control and I don't have rigid tapping -- my spindle is an AC motor and is not able to orient (think DC motor with encoder) which is a requirement for rigid tapping. The tap holder I use is not a tapmatic, it is simply a floating tap holder. It has the ability to extend in both the forward and reverse direction to compensate for a feed rate that might not be exactly in tune with the thread pitch. Rigid Tapping doesn't have this requirement any chuck that can hold a tap will work.

That aside, the ability to just do simple tapping would be huge!

[Helical]

On a mitsubishi controller G84 is an automatic tapping cycle with spindle reverse. Same goes for Fanuc controllers, these work with a floating tap holder to allow a bit of Z axis freedom.

[jbraun]

For linuxcnc G84 with G20 and 1/4-20 tap :

M3 S400
G84 Z-0.5 R0.1 F20 (400 rpm cw to depth, 400 rpm ccw retract at same feed rate)

I worked in 2 shops and G84 with floating holder was the most used method for mills ..... this with machines capable of true rigid tapping.
Whether that's the norm in industry I surely don't know.

[luvtofish]

Yep, Yep. We need this feature added please!

Thanks

Dan

[luvtofish]

Opened following Feature Request:

https://github.com/FreeCAD/FreeCAD/issues/8018

Dan

[GeneFC]

Opened following Feature Request:

Your feature request seems to include all the detailed movements required for the complete operation. For a typical canned cycle the CAM program sends all the required parameters via the Gxx command, and then the CAM program is done. The machine controller handles all the details of halt, dwell, reverse, retract, etc.

Not saying it cannot all be done in CAM software instead of controller software/firmware/hardware, but this would be an extension to the usual practice. It also likely means the CAM software (Path WB) would need to handle a number of variations for different machines.

Gene

[luvtofish]

Opened following Feature Request:

Your feature request seems to include all the detailed movements required for the complete operation. For a typical canned cycle the CAM program sends all the required parameters via the Gxx command, and then the CAM program is done. The machine controller handles all the details of halt, dwell, reverse, retract, etc.

Not saying it cannot all be done in CAM software instead of controller software/firmware/hardware, but this would be an extension to the usual practice. It also likely means the CAM software (Path WB) would need to handle a number of variations for different machines.

Gene

Yes, most controllers will handle the spindle functions by virtue of the G84 call. CAM would supply the g codes (G84/G80), xyz movements and could also be coded to assist with computing the feed-rate by capturing a user entered spindle speed.

I will edit the request to be more clear as I wasn’t looking for CAM itself to handle all those functions.

Really shouldn’t be to difficult to add this to Path.

[karlnick]

Tapping cycle would be useful for me too. Trying to get a more complete list of "hole" making, looking into Linuxcnc:

Useful for threading:

• G33 Spindle synchronized motion, may be used to produce thread.
• G33.1 Rigid tapping, this is useful for me.
• G74 Left-hand Tapping cycle, most certainly useful for some.
• G74 Left hand cycle, dwell ought to be useful for some though probably rare.
• G76 Is for lathe.
• G84 As discussed here is right hand cycle, dwell.

Drilling:

• G73 Drilling cycle with chip break. Useful and implemented by selecting "peck" + "Chip Break".
• G81 Drilling cycle. Useful and implemented by neither selecting "Peck" nor "Dwell".
• G82 Drilling Cyclle, Dwell. Implement by selecting dwell.
• G83 Peck Drilling Cycle. Implemented by selecting "Peck" but not "Chip break".

Reaming? Boring:

• G85 Boring Cycle, Feed Out. Not implemented.
• G86 Boring Cycle, Spindle Stop, Rapid Move Out. Not implemented.
• G87 Back boring cycle. Not implented in Linuxcnc nor in Freecad.
• G88 Boring Cycle, Spindle Stop, Manual Out. Not implented in Linuxcnc nor in Freecad.
• G89 Boring Cycle, Dwell. Feed Out. Similar to G82 but retract at feed rate instead of rapid move.

Would guess it would be rather straight forward to implement most of them except G76 for lathe. Though not sure how hard it is to figure out and add suitable check boxes and add conditions in code depending on selected check boxes sot that correct G-code is chosen possible implemented with several g-codes if direct support is missing. Or maybe I think wrong something more need to be added.