[makbari]

Does anybody knows how can I fix my tapping problem?!

I work with Mazak 640M and use G84 for tapping after couple holes keep breaking,
I use deffernt kind of tap like Spril point, Sprilt flute even form tap,

I used form tap and used S800 F40. for 1/4-20 and cheaps stick to tap after doing some holes and will break,

I used Spril point, Sprilt flute too with different speed and feed but still keep breaking after some holes, what is wrong?

I am using Coolant for lubrican,

Thnaks Guys

[CNCRim]

Have you try to slow down to S300?

[makbari]

I have try slow speed with Spril-point and Spril flute one but Form tap supose to do faster, I am not sure if there is any parameter on Mazak that I have to set or not?!

[CNCRim]

Well, whatever you did not work, so it is not right. If you program with Mazatrol then yes there is parameter.... but G-code no.

[metalworkz]

Hello,
It sounds like the tap is getting too hot and the chips are bonding to the tap. Perhaps the coolant is not a good cutting fluid for tapping aluminum, so why not try a regular tapping fluid and possibly a fluid made specifically for aluminum? Are the holes the correct size for the taps being used(ie 1/4-20 cut usually .201" dia and for the roll tap the hole needs to be bigger....228" dia. if I remember correctly) Also are the chips being cleared from the hole and how deep are the threads you are cutting, or are the holes blind holes? It all has a bearing on how the tapping will work.

[dertsap]

you don't say what depth or what type of aluminum your cutting so it's impossible for you to get the right answer to your question , if your tapping very deep then you may need to peck tap it , also if your dealing with soft gummy aluminum then once again you may need to peck ,
you could check the drawing to see what class of thread you need to cut then drill at the top of the tolerance ,
what brand of taps are you using

[makbari]

I am using Nachi Tap HSSE, it is AL 6061, 1/4-20 2B, hole size drill#7,
with Coolant, I am not using Mazatrol code, I am using G-code, and Mastercam to make program, I know there is some parameter for Mazak but not sure if has to be set, and do not know about them what supose to be?!

[dertsap]

you didn't mention the depth but if your depth is above 2/3 to 1 1/2 times dia then min and max hole size is .202-.207 ,
if your above 1 1/2 to 3 times dia then the hole size can be .204-.210
min/max tolerance for a 2b thread

[Superman]

G84, is that a "Rigid Tap Cycle" for the mazak

When, in the cycle are the taps breaking ?

If not a rigid tap cycle
How are your tap being held ?
Are you using a floating holder to allow for the stopping and reversing of the spindle ?

If a thru hole, gun taps may last longer and be a bit stronger

[psychomill]

Depending on your parameter setting (Yes, there is a parameter for G code).... G84 is rigid tapping but NOT synchronoized. You need a floater.

You can try one of 2 things here......

add code if you want to keep using G84

G84 Z-.5 F.05 H1

or change to synchronized tapping code...

G84.2 Z-.5 F.05

In either case, you'll need to use the tap pitch as the feed and not the calculated feed like you have it.... unless you want to use a floater...
I normally do not change the parameter for G84. I generally use G84.2 and that way, I maintain the option of using either tap cycle types if I want (to float or not to float)....

[steveo]

I use G84 all the time in aluminium. higher end sfm the better. thicken your coolant aluminium does not like water. follow your tap manufacturer correct sfm

[hnevans]

Depending on how many parts that you have to run, I recommend just drilling to desired depth and just tapping maybe .500" deep. Afterwards, hand tap to finish depth. This allows the tap be on location and square to surface with minimal hand tapping. Also, there aren't any broken taps to remove. I would run tap at 10 times what ever tpi is and use F10. for feed. For example 1/4-20 run at 200rpms and F10., 1/2-13 run at 130rpms and F10. I am certain this is correct, but I'm at home and unable to ensure that I am right. Therefore, I also advise to try this in a test piece first. It also wouldn't hurt to put an optional stop M01 in program before the tap runs and just add some Rapid Tap or other cutting oil in the holes. I have done this before and it helps as well. I would use a siral flute CNC tap if available. Formula for Feed = pitch X RPM. Therefore, when running other taps use the Feed formula given with 10. as feed and solve for RPM. For example a 1/4-20 would be 10=.05(x) solve for x. With "x" being the RPMs.

[espron]

Are you tapping on center or using a mill/drill pot ? Could you have bumped your machine ? May be worth puting a clock on the chuck and clocking the pot to make sure, if you have tryed different taps sounds like its being loaded up for some reason if you have correct hole size and speeds and feeds give or take .

[makbari]

Problem has been solved, Ii was Post processor

[makbari]

Does anybody now what is the best Feed and speed for reamering the Aluminum 6061 for 1/4, 5/16, 3/8, 1/2 hole size, and how much hole size suppose to be (the best one)?, depth is almost 1.0"
also how can I make it tight or lose with feed and speed,

Thanks