Drill Depth vs. Tap Depth

[richardsalzman]

I am new to rigid tapping and getting ready to tap a few holes in a 5/8" flat aluminum plate that I will be using as a fixture plate.  I will be tapping 1/4 x 20 holes and trying to establish the correct hole depth vs tap depth.  I am using the GWizard calculator and while the software is ok, the documentation can be convoluted and contradictory.

I plan to use a bottom chamfer tap, GWizard indicates that the drill depth should be .189" deeper than the tapped depth for a bottom chamfered tap (see below).  Gwizard also indicates that the drill depth for a plug tap should be .339" deeper.

This is confusing because the documentation suggests that bottom chamfer taps have no value for CNC (see below).  I am new to this so most important; I would like to know if the .189" additional depth for a bottom chamfer tap make sense?

While programming the tool paths, I had to keep in mind that in Fusion (Design), the hole command indicates hole depth NOT including the tip of the drill, but in CAM, it appears that the height tab DOES include the depth to the tip of the tool.

Richard

[a.laasW8M6T]

Hi Richard

The bottoming taps talked about there are Hand taps like this

They have straight flutes and do a poor job of Chip evacuation.

For any power tapping(CNC or other) operation in Blind holes you should be using Spiral Flute taps like this

The spiral Flute taps still have some chamfer on the end a cannot create threads right to the bottom of the hole.

Typically they have a 3xLead chamfer, though this does vary depending on exactly which tap you have.

I just run my taps right to the bottom of the hole, this is safe to do with rigid tapping

I have my setting like this for the drill

and for the Tap

I also notice your chamfer is too small, I like to go 0.5mm(0.02in) larger than the tap major diameter, so 0.25+0.02=0.27

0.27-0.202=0.068

0.068/2 =0.034 for the chamfer size

I also prefer to chamfer before tapping as chamfering afterwards can push burrs into the threads

see attached file

[richardsalzman]

Andrew,

Thanks for all the nice tips.  Perfect!  

With respect to taps.  I am using machine taps.  I ordered one with a plug chamfer and one with a bottoming chamfer so I could get closer to the bottom of the hole (see below).  I have not experimented with the bottoming chamfer tap yet.

I took the Fusion file you shared with me and added a 3 second dwell just for testing purposes.  I ran the gcode from this file and measured how deep the tap went down.  For testing, I entered G52 z3 and measured how far the tap reached against a 123 block (see attached).  I measured a depth of approximately .628".  I understand that the hole depth in the Fusion file is .525" and that the tip of drill (135-degree point) extends about .05".  Therefore the depth to the point of the drill should be about .525" + .05" = .575".  So why is the drill reaching a depth of .628"?  An additional .050 inches.

Any thoughts... Richard

[a.laasW8M6T · Accepted solution]

Hi

The drill point is 0.0414 for that size drill, so fusion drills to -0.5664 which is 0.525+0.0414.

If the tap is going deeper than what is programmed it has to be a machine/controller problem

Its only being commanded to go to -0.525

N350 G84 X1.582 Y-1.6 Z-0.525 R0.1 Q0.05

My understanding of Rigid tapping is that the Spindle rotation is measured by the Encoder, and then the controller try's to follow with the Z axis as closely as possible

If you are overshooting In Z You must need to tune the spindle acell/decell parameters for the tapping 

seems like parameter 82 might need to be adjusted

[richardsalzman]

All Set.  I tested it by tapping in the air.  When tapping in the aluminum... it worked great.

Thanks so much for all your help!

Richard