Thread: Tapping help!

So I've done tapping with my CNC a ton of times and have never had this issue.

I'm trying to tap a 5/16-18 hole.

I'm using a 0.257 drill and then a 5/16-18 bottoming tap because i don't have a lot of through clearance in the 0.7 thick plate.

I tried using a SFM of 90, and it looked like the tap just bored the already drilled hole with no threads as shown:



So then I slowed the SFM down to 70 and got the exact same results.

I then manually tapped one of the holes (I have 150 to do), and it came out fine!

There's something very obvious that I'm missing here....


Thanks,

Alex

I'm using a HAAS VF-3YT

Any chance you're tapping with a non-floating holder and using a rigid tap cycle with the wrong feed rate?

You can help the forum help you by posting the code.

QB

Originally Posted by PixMan

Any chance you're tapping with a non-floating holder and using a rigid tap cycle with the wrong feed rate?

Yes, I'm tapping w/ a non-floating holder and using a rigid tap cycle.
I used G-Wizard for my speed/feed. I think that has to be the problem. Maybe even because it's a bottoming tap, that I'm getting the wrong feeds/speeds.

I don't know if there's a seperate formula I should use for a bottoming tap or if someone just has a good idea of what I should use for a 5/16-18 bottoming tap into a 0.7" thick piece of 6061 w/ a 0.257 hole?

Originally Posted by Question Boy

You can help the forum help you by posting the code.

QB

N1726 T16 M6
N1728 G0 G90 G54 X.625 Y-.75 A0. S611 M3
N1730 G43 H16 Z.1 M8
N1732 G94
N1734 G99 G84 Z-.7 R.1 F152.8
N1736 X2.125
N1738 X3.625
N1740 X5.125
N1742 X6.625
N1744 X9.625
N1746 X11.125
N1748 X12.625
N1750 X14.125
N1752 X15.625
N1754 X17.125
N1756 X18.625
N1758 X20.125
N1760 X21.625
N1762 X1.375 Y-1.5
N1764 X2.875
N1766 X4.375
N1768 X5.875
N1770 X7.375
N1772 X8.875
N1774 X10.375
N1776 X11.875
N1778 X13.375
N1780 X14.875
N1782 X16.375
N1784 X17.875
N1786 X19.375
N1788 X20.875
N1790 X.625 Y-2.25
N1792 X2.125
N1794 X3.625
N1796 X5.125
N1798 X6.625
N1800 X9.625
N1802 X11.125
N1804 X12.625
N1806 X14.125
N1808 X15.625
N1810 X17.125
N1812 X18.625
N1814 X20.125
N1816 X21.625
N1818 X1.375 Y-3.
N1820 X2.875
N1822 X4.375
N1824 X5.875
N1826 X7.375
N1828 X8.875
N1830 X10.375
N1832 X11.875
N1834 X13.375
N1836 X14.875
N1838 X16.375
N1840 X17.875
N1842 X19.375
N1844 X20.875
N1846 X.625 Y-3.75
N1848 X2.125
N1850 X3.625
N1852 X5.125
N1854 X6.625
N1856 X8.125
N1858 X9.625
N1860 X11.125
N1862 X12.625
N1864 X14.125
N1866 X15.625
N1868 X17.125
N1870 X18.625
N1872 X20.125
N1874 X21.625
N1876 X1.375 Y-4.5
N1878 X2.875
N1880 X4.375
N1882 X5.875
N1884 X7.375
N1886 X8.875
N1888 X10.375
N1890 X11.875
N1892 X13.375
N1894 X14.875
N1896 X16.375
N1898 X17.875
N1900 X19.375
N1902 X20.875
N1904 X.625 Y-5.25
N1906 X2.125
N1908 X3.625
N1910 X5.125
N1912 X6.625
N1914 X8.125
N1916 X9.625
N1918 X11.125
N1920 X12.625
N1922 X14.125
N1924 X15.625
N1926 X17.125
N1928 X18.625
N1930 X20.125
N1932 X21.625
N1934 X1.375 Y-6.
N1936 X2.875
N1938 X4.375
N1940 X5.875
N1942 X7.375
N1944 X8.875
N1946 X10.375
N1948 X11.875
N1950 X13.375
N1952 X14.875
N1954 X16.375
N1956 X17.875
N1958 X19.375
N1960 X20.875
N1962 X.625 Y-6.75
N1964 X2.125
N1966 X3.625
N1968 X5.125
N1970 X6.625
N1972 X9.625
N1974 X11.125
N1976 X12.625
N1978 X14.125
N1980 X15.625
N1982 X17.125
N1984 X18.625
N1986 X20.125
N1988 X21.625
N1990 X1.375 Y-7.5
N1992 X2.875
N1994 X4.375
N1996 X5.875
N1998 X7.375
N2000 X8.875
N2002 X10.375
N2004 X11.875
N2006 X13.375
N2008 X14.875
N2010 X16.375
N2012 X17.875
N2014 X19.375
N2016 X20.875
N2018 X.625 Y-8.25
N2020 X2.125
N2022 X3.625
N2024 X5.125
N2026 X6.625
N2028 X9.625
N2030 X11.125
N2032 X12.625
N2034 X14.125
N2036 X15.625
N2038 X17.125
N2040 X18.625
N2042 X20.125
N2044 X21.625
N2046 G80
N2048 G94
N2050 M5
N2052 G91 G28 Z0. M9
N2054 A0.
N2056 M01

not sure if it's really going to help in this case, but here you go!

I would check tool setup. many machines if you input 5/16-16 thread accidentally in tool data instead of 5/16-18 some machines will give "no suitable tool error message". obviously if feed rate is different than tap somethings got to give

1/18=.05556*611 rpm=33.947 IPM. Really, 'tis not that difficult to see visually if feed is correct. Not hard to calculate either. Feed's way fast, surprised you still have a tap left in the holder...TG it's Aluminium.

so, the feed rate I have listed in the code above is what G-Wizard initially recommended. I thought that was a bit high, so I went with something more conservative and that's what brought me to my initial problem.
just now I decided maybe I should've gone with the initial recommended feed/speed, so I changed that and it broke the tap into the material. Which I'm guessing has to do with the fact that a normal tap could've handled it fine... a bottoming tap needs a slower feed..

The type of tap does not matter to the RPM/IPM equation. Just thought I'd point that out. Hope this helps. Happy Tapping to you, Sir!!!

Originally Posted by John Willliams

The type of tap does not matter to the RPM/IPM equation. Just thought I'd point that out. Hope this helps. Happy Tapping to you, Sir!!!

Thanks John, that does help. I'll see what I can do after I get this broken tap out

Recalculating the feed rate, that was totally my fault. I some how used the wrong thread pitch, giving me that ridiculously high number. Stupid mistake.

Originally Posted by clemens1292

so, the feed rate I have listed in the code above is what G-Wizard initially recommended. I thought that was a bit high, so I went with something more conservative and that's what brought me to my initial problem.
just now I decided maybe I should've gone with the initial recommended feed/speed, so I changed that and it broke the tap into the material. Which I'm guessing has to do with the fact that a normal tap could've handled it fine... a bottoming tap needs a slower feed..

Your feed rate is governed by the thread lead. I doubt you have tapped a ton of holes.

Originally Posted by clemens1292

so, the feed rate I have listed in the code above is what G-Wizard initially recommended. I thought that was a bit high, so I went with something more conservative and that's what brought me to my initial problem.

I like concervitism (werd?)

But when it comes to "feed" on a tap - there isn't concervative, nor proud.
Only "correct".

I came up with the same feedrate as John.
But I have never programmed rigid in IPM before.


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

I am Ox and I approve this h'yah post!

Got it guys. Thanks.

Okay, bear with me here. I have tapped a decent amount of holes, but by no means as many of most of you probably have. I've also never attempted to tap this many at a time. I'm learning.

I used the right feed/speeds. The first couple holes come out great and then it appears the tool starts wearing pretty fast up until about the 20th hole, where the tool then breaks.

My coolant is perfect. The hole size is right.

It's a NATC HSS tap.

Any ideas?

The hole on the far left is the threades hole right before breaking. And on the right, is obviously the broken tap. The middle hole isn't related.

Are you still using a bottoming tap? Hard to tell now that it broke, but it looks like it was a straight fluted tap.

If you have problems getting the tap out ,try a paste of Alum. Supposed to eat thru the steel and not harm the aluminum. I haven't tried it myself, I will if I ever break another one. Many of the taps I use are very small,1/64 2/56 as examples. Alum is supposed to be sold in super markets in the spice aisles.McCormick is one brand. I bought a pound on line because our stores don't carry it.Google "alum" /tap removal.
mike

I would not use a bottom tap in this situation. They are not meant for initializing threads. Might I suggest the Emuge brand "blue stripe" tap? This is what is called a "modified bottom" tap. It is spiral fluted, achieves full thread at about 2 leads or so, and will eject the shavings from the hole. You can take it right to the bottom of a blind hole if rigid tapping and it is "almost" a bottom tap. IMHO, 5/16"-18 is where these taps really become viable, 1/4"-20 can be troublesome if tapping deep. They are expensive, but what you are doing now is even more costly. No reason why 20 holes would be the life expectancy of this one in aliminium. Just judging from your program, this is a sizable chunk of aluminium that somebody is going to eat unless your customer will allow helicoil repair. Whether or not you have tapped tons of holes in the past, there appear to tons of holes in just this one part.

Not to be an ass, trying to be helpful here, feedrate versus RPM is NOT something you can fiddle with or make judgement calls or estimates. Whatever the rpm you choose, by whatever means and for whatever reason, the feedrate MUST correspond according to the formula I gave above. ESPECIALLY if you are rigid tapping, there is NO WIGGLE ROOM HERE.


Please let me know how it turns out.
John

Originally Posted by Dave K

Are you still using a bottoming tap? Hard to tell now that it broke, but it looks like it was a straight fluted tap.

These are the taps I'm using:

Stop trying to get it done with cutting taps and get yourself a quality roll form tap! That's a HAND tap and there's no chip control. That's why it's breaking.

Just be aware that hole size is larger for those and size control is critical to get the percentage of full thread form that's required.

Originally Posted by John Willliams

I would not use a bottom tap in this situation. They are not meant for initializing threads. Might I suggest the Emuge brand "blue stripe" tap? This is what is called a "modified bottom" tap. It is spiral fluted, achieves full thread at about 2 leads or so, and will eject the shavings from the hole. You can take it right to the bottom of a blind hole if rigid tapping and it is "almost" a bottom tap. IMHO, 5/16"-18 is where these taps really become viable, 1/4"-20 can be troublesome if tapping deep. They are expensive, but what you are doing now is even more costly. No reason why 20 holes would be the life expectancy of this one in aliminium. Just judging from your program, this is a sizable chunk of aluminium that somebody is going to eat unless your customer will allow helicoil repair. Whether or not you have tapped tons of holes in the past, there appear to tons of holes in just this one part.

Not to be an ass, trying to be helpful here, feedrate versus RPM is NOT something you can fiddle with or make judgement calls or estimates. Whatever the rpm you choose, by whatever means and for whatever reason, the feedrate MUST correspond according to the formula I gave above. ESPECIALLY if you are rigid tapping, there is NO WIGGLE ROOM HERE.


Please let me know how it turns out.
John

Great information. I'll look into the blue stripe tap and let you know how it goes. I think I'm going to step back for today and get back into this tomorrow..

Thanks again for all the help.