M2 x 0.4 Taps

[chriswlbr94]

Hey all, I had success with the help from you guys last time, so I'm hoping I can get some knowledge on this as well. I am tapping with some M2 x 0.4 taps and they keep breaking I can get one hole tapped, and then the next one snaps on me. I have the holes pre drilled thru, and it is the correct dimension hole for this size tap. I'm only running this cycle at 350 RPMs and a feed rate of 5.511 IPM with rigid tapping. I created a new tool in MC with the IPT, diameter, etc. of the tool properties. Any idea why they keep breaking on me? Is it poor chip removal and they keep binding? Thanks  

[Manofwar]

What material, depth, and machine are you running this on? Peck tapping may help out with this issue, as well as using a better lubricant (such as Moly tapping fluid.)

[#Rekd™]

Do you have a floating tap holder or is it rigid in an er collet chuck? Blind or through hole? Type of tap? 

[chriswlbr94]

The material is 6061 aluminum, and the depth I'm tapping is only about .32" deep, with a thru-hole drilled prior. I am using a HAAS DM-1 with rigid tapping, and just using the coolant/fluid that we have mixed for our aluminum milling. It is a not a floating tap holder and I have tried using both a spiral flute and straight flute tap. Thanks again guys.

[Manofwar]

That's pretty deep for that size tap. I would switch to peck tapping. Most taps at that size only have 7mm of flute. So the odds are high that the upper portion of the tap is blocking the coolant from doing it's job. As well as the chips from escaping (on the spiral tap.) If you have tapping fluid, use it.

 

Normally at this size I would use a roll tap to avoid the issue of chip pack, and peck tap to depth. Takes a bit longer, but better then breaking taps constantly.

[chriswlbr94]

46 minutes ago, Manofwar said:

That's pretty deep for that size tap. I would switch to peck tapping. Most taps at that size only have 7mm of flute. So the odds are high that the upper portion of the tap is blocking the coolant from doing it's job. As well as the chips from escaping (on the spiral tap.) If you have tapping fluid, use it.

 

Normally at this size I would use a roll tap to avoid the issue of chip pack, and peck tap to depth. Takes a bit longer, but better then breaking taps constantly.

Thank you for that suggestion, I will give that a go. I just ran the part again and used our tapping fluid instead of the machine coolant, and that worked. Not sure if that was just luck though lol. I'm unfamiliar with a peck tap, in MC i only see the peck drill and tap options.

[Manofwar]

It's been awhile since I used Mastercam. But I believe this has to do with whether the post supports it. You could add it to the post if you really wanted it as an option. Video on Youtube shows how it is done here. If you just need it once, the machine should support it and you can just edit the G84 line with a 'Q' telling it how deep you want per cycle.

 

[Jobnt]

Since your hole is through chip buildup at the bottom should not be an issue. The tap is about 4x the dia so that's moderately deep for that size tap. 

What size drill are you using? Not all drill charts are the same: Some based on 70% thread engagement, some at 75% etc. There are calculators available to calculate the thread engagement.

Is the minor dia spec'd on the drawing? If not you can make it a few thou bigger and that might help make it through using the standard coolant. 

[Newbeeee™]

If cut tapping...you need bright (uncoated) finish tap. Clocked in to run zero runout.

Spiral point tap geometry (which is stronger and will push the swarf through).

Faster RPM - 1500 minimum.

Coolant strength at 10%. 

 

But preferably, roll tap it....

[Jobnt]

23 minutes ago, Newbeeee™ said:

Faster RPM - 1500 minimum.

+1 to this. ^^^

[crazy^millman]

On 2/23/2023 at 1:48 PM, Newbeeee™ said:

But preferably, roll tap it....

Winner Winner Chicken Dinner.

[jpatry]

On 2/23/2023 at 11:22 AM, Manofwar said:

Normally at this size I would use a roll tap to avoid the issue of chip pack

Yep, form taps are a glorious thing.

Only major thing  to worry about is thinwall bulging, which is easily solved by getting the tapping done before final wall finish in the relevant areas

Edited April 9, 2023 by jpatry

[Colin Gilchrist]

Looking at the numbers, a Metric Pitch of 0.4mm = 0.015748031496063" per tooth.

I always try to adjust my RPM to hit a Tapping Feed Rate which isn't rounded (or is rounded very, very little), to help avoid accumulated pitch errors.

I agree with tapping faster, but 0.015748031496063" is a tough pitch to find the right RPM to cut at, because RPM is only specified in integer values. (Can't do decimal values on the commanded RPM.)

For this pitch, I believe 889 RPM is perfect. That would give you a tapping feedrate of 14.0000000 Inches per Minute. Or you could double the RPM to 1,778, and tap at 28 IPM.

I would look to Emuge for taps. Is the hole truly "thru", with ample clearance on the other side of the hole to push the chips through? If so, a Spiral Point Tap would work, just keep in mind that it won't "pull" the chips out from the hole, but will "push" them through.

Form Tapping would give great results, or look to a "Spiral Flute Tap" to pull the chips.

If I have the option, I like to run the Pulse Jet lubrication option on Haas machines, and fill the reservoir with Aluminum Tap Magic, and just use the Pulse Jet for the tapping operations, but use regular coolant for everything else. The other option (as has been mentioned in this thread) is to use regular coolant, but make sure your concentration level is at 10% or above.