Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

steel tapping


elraiis
 Share

Recommended Posts

Hi guys,

can anyone advise me what rpm to use for tapping mild steel! M3, M4, M5 TAPS.. DISTROYED 4 TAPS SO FAR I CAN'T FIGURE OUT WHATS WRONG. my ignorance no doubt but we hardly touch steel and ss. mostly brass and alum.. any advise is greatly appreciated please.

p.s we increased to coolant concentration hoping to help and resolve this problem but no good. called the guy who sold us the taps and he was even suggesting a faster rpm than the one i actually used.. tried what he said and it lead to a faster catasrophy.. i MUST be doing something wrong. and this is no hard steel.. 1020 grade. soon SS 304 is coming and i wonder... biggrin.gif

thanks in advance all..

Link to comment
Share on other sites

Use best brand taps. ( eg Prototyp )

 

Use spiral tap.

 

Over drill the core drill size by ~~ .05-.1mm it will result to 80% to 70% thread which may still be under ur specs.

 

Use the right cutting speed ( not too slow!)

 

Check ur machine parameter is set for syncro tap,

Otherwise use a floating tap holder and reduce the feed to ~95%

 

You will be alright!

Link to comment
Share on other sites

quote:

Blind hole but i left almost .120" between depth of the drill and that os the tap in case chips are stuck in

.120 deeper? I would allow more than that. That's almost the length of the drill point of a M5 tap drill, which means you didn't leave any clearance. If you're not using the type of tap that sends the chips spiraling out of the hole, then you're cramming the chips into that .120 "clearance."

 

Sorry I can't help with speeds and feeds. Those were set in the libraries years ago and I pay no attention to them any more.

 

Thad

Link to comment
Share on other sites

the taps am using are spiral yes and teh .12" gap betwen the tap and the drill i meant to say if in my program my tap z value is -.5 my drill z value is -.620 but a very important point you raised.... cutting fluid! that makes sense but how is the cnc machine going to do that! sorry but i don't get it.

 

roll taps! i didn't think of trying that i thought cutting would be the right choice but u know what.. i'll try that tomorrow hoping to have it work..

 

i can't really increase the hole size before the tap as that would, as you have guessed, make the tap out of the tolerance required by the client!

 

thanks for the help guys.. i still am not sure what i am supposed to do though. and i hate the idea of guessing until i get it right.. i'll have a graveyard of taps. biggrin.gifwink.gif i'll c if forming tap combined with floating tap holder would make the difference..

 

thanks all again

Link to comment
Share on other sites

A suggestion for any tapping is to set feed per rev before tapping cycle so that your feedrate = programmed pitch , then the operators can adjust RPM in the program without affecting the pitch

 

***DON'T FORGET G94*** turn feed per minute ON as most millers like feed per minute or your next feed move on the part wil be v________e________r________y quick

 

Core drilling sizes for spiral taps are very different to roll taps ( roll tap core sizes must also be tightly controlled )

 

When tapping into SS-304 , take the core sizes to just under the highest size permitted.

 

Cutting speed for tapping 1020 @ 7-10 m/min

for M6 * 1.0p = S300 > S600 ( can go higher )

can use coolant or compound

 

Cutting speed for tapping SS-304 @ 4-7 m/min

for M6 * 1.0p = S200 > S400 ( can go higher )

use compound

 

Spindle is NOT started at RPM line as to keep tool in sync, even if it is toolchanged

 

example code for OKUMA

G15 H1

G0 X0. Y0.

S300

G71 Z2.

G95

M00 ( BLOWN DOWN and APPLY CUTTING FLUID )

G284 Z-.5 R.3 F.04 M53 ( g-code starts RH rigid tap cycle )

X1. Y0.

X1. Y1.

X0. Y1.

G00 ( or G80 = cancel cycle )

G94 (**** note ****)

M9

M5

G30 P1

M01

Link to comment
Share on other sites

floating tap head combined with spiral flute tap(something of quality like dormer or emuge) and lots of coolant. I tap holes all the time with no problem. as check that you don't have your depth messed up. Also because it is mild steel it is gummy, so i recomend drilling it a little on the big side if you don't need 75% thread engagement. Good luck let me know how it works out.

 

Keith

Link to comment
Share on other sites

hi guys.. and thanks to all of you. yes it worked today. the spiral flute expensive taps finally cut the threat after taking rpm down to 100rpm! banghead.gif roll tap was the real answer. we gave back all those spiral flutes cutting taps and got standard forming taps and guess what... i was stunned but it worked perfect on our milling machine. 1500rpm... much faster and seriously... i would have never guessed to use forming taps on steel. thanks alot to everyone i really appreciate it.

peace

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...