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....
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.
Yes, I'm tapping w/ a non-floating holder and using a rigid tap cycle.
Originally Posted by PixMan
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
not sure if it's really going to help in this case, but here you go!
N1726 T16 M6
N1728 G0 G90 G54 X.625 Y-.75 A0. S611 M3
N1730 G43 H16 Z.1 M8
N1734 G99 G84 Z-.7 R.1 F152.8
N1762 X1.375 Y-1.5
N1790 X.625 Y-2.25
N1818 X1.375 Y-3.
N1846 X.625 Y-3.75
N1876 X1.375 Y-4.5
N1904 X.625 Y-5.25
N1934 X1.375 Y-6.
N1962 X.625 Y-6.75
N1990 X1.375 Y-7.5
N2018 X.625 Y-8.25
N2052 G91 G28 Z0. M9
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!!!
Your feed rate is governed by the thread lead. I doubt you have tapped a ton of holes.
Originally Posted by clemens1292
I like concervitism (werd?)
Originally Posted by clemens1292
But when it comes to "feed" on a tap - there isn't concervative, nor proud.
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!
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.
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.
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.
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
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.