Busting off taps $#@$#@

[Bob W.]

I have broken a few taps now and I am getting a little frustrated about it. Last night I broke a 6-32 tap and tonight I broke a 10-24 tap, the first time I had ever used it. What might I be doing wrong? The taps are spiral fluted, bright finish and run at 300-450 rpm in 6061 aluminum. My mill is a Haas Mini Mill ('05) with the rigid tapping option and the taps are held firm in ER16 collets. It appears that the mill's feed and spindle are not perfectly in sync, but that is just a guess. I didn't have a lot invested in this particular part but that might not be the case next time. Any ideas?

 

Thanks,

Bob

[Flycut]

EDIT: Answering too fast.

You in fpm or fpi?

Can you show us some code?

[Bob W.]

I am using rigid tapping without a floating tap holder. The tool is held firm in an ER16 collet with standard flood coolant and the code is as follows:

 

N124 T2 M6

N126 G0 G90 G54 X3.2 Y-.2125 S480 M3

N128 G43 H2 Z.1

N130 M8

N132 G99 G84 Z-.35 R.1 F20.

[Guest CNC Apps Guy 1]

I use IPR (G95) when tapping myself AND I use Peck Tapping when /if possible. To see if you machine wil peck tap, create a tapping cycle and put a "Q" with a value (ex. Q.125) and see if it pecks.

 

Here's my "ptap" and "pcanceldc", for a Mori Seiki (Based on MPMaster), modify for your situation;

 

code:

---

ptap            #Canned Deep Hole Tap Cycle

pdrlcommonb

#RH/LH based on spindle direction

if use_pitch, pbld, n, "G95", e

if use_pitch = 0,

[

n, *sm05, e

n, "M29", *speed, e

pcan1, pbld, n, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout, *peck1,

prdrlout, dwell, *feed, strcantext, e

]

else,

[

if met_tool, pitch = n_tap_thds # Tap pitch (mm per thread)

else, pitch = 1/n_tap_thds # Tap pitch (inches per thread)

n, *sm05, e # Force Turn Off Spindle

n, "M29", *speed, e # Set Rigid Tapping Active

pcan1, pbld, n, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *peck1, *pitch, !feed, strcantext, e

]

pcom_movea

tapflg = 1

---

code:

---

pcanceldc       #Cancel canned drill cycle

result = newfs (three, zinc)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

if cool_zmove = yes & (nextop=1003 | (nextop=1011 & t<>abs(nexttool))), coolant = zero

pcan

pcan1, pbld, n, "G80", scoolant, strcantext, e

if use_pitch & tapflg = 1, pbld, n, *sg94, e

pcan2

tapflg = 0

---

[Flycut]

Is this a thru hole?

.350 isn't very deep shouldn't have to peck.

Just remembered ipr is not an option on our haas.

Where's you M29?

[Bob W.]

M29? Whats that? I don't see one anywhere.

[Bob W.]

I guess I should add that I am new to CNC machining and I bought the Haas because I have wanted one for some time. I have several years of manual machining experience. By no means am I a CNC expert

[DavidB]

I never used A HAAS but is there a code that preps the sync between spindle and feed?

 

My Makino needs M135 before the G84

 

HTH

 

[ 02-08-2006, 12:12 AM: Message edited by: DavidB ]

[Flycut]

My apologies... I think I work with too many different controls.

M29 must be on the hardinge at my weekend job.

I can't seem to find anything wrong with what you have so far.

[Flycut]

Have a look over here you might find something that'll help you.

 

fear of tapping

[Bob W.]

I had a look at my machine and it appears that the rigid tap feature was not turned on. I paid for it, so it should have been Oh well, I'll bet that makes a bit of a difference. It is on now and I will be in touch with my Haas dealer soon. Thanks for the help.

 

Bob

[DavidB]

Your code has F20. What tap was that for? The feed must be relievent to the Pitch.

 

Also make sure your tapping position is the same as your drilling position?

When doing tapping I always copy the drilling op paste it then change the drilling method to tapping, also select the correct Tap.

 

This way if I change the position of the point for drilling the Tapped hole is also linked to the same point.

 

HTH

[MercFan]

I know when I started tapping on my Haas VF3 I wound up with just a bunch of stripped holes.

 

Turns out MasterCAM will not allow posting of rpms below certain feeds. My minimum spindle was set at 100, and I needed 60rpm for my feed.

 

I don't know if the same it true for feeds...

 

But to give you and idea, I run a M12 tap at 60rpm (since I fixed that damn parameter in masterCAM) I don't use pecking or anything. Standard tapping cycle in mastercam. The tap is a helical flute machine tap.

 

Everything I give is in mm, but here's my setup.

M12x1,75 tap

60rpm

105mm/min feed

 

Feed = rpm x pitch

105 = 60 x 1.75

[Bob W.]

Problem solved. I turned on rigid tapping in my machine and it tapped 40 holes perfectly. I guess when one orders a feature on their mill, such as rigid tapping, one shouldn't take for granted that the factory actually turned it on. Oh well, lesson learned. There is a definite difference in the way it taps holes now and if I had more experience I would have caught it right away. Thanks again for the help.

 

Bob

[Guest]

Mercfan

quote:

---

Turns out MasterCAM will not allow posting of rpms below certain feeds. My minimum spindle was set at 100, and I needed 60rpm for my feed.

---

It is not Mastercam that limits your speed, the minimum spindle speed is set in your post. You do have to be aware of the minimum spindle speed your machine can run also

 

code:

---

max_speed   : 8000  #Maximum spindle speed

min_speed : 50 #Minimum spindle speed

---

I don't know if this function has been passed over to the machine def yet.

[MattW]

On a somewhat related note, you do not need an M3 command when rigid tapping on a Haas (and maybe other tools), the G84 turns the spindle on and off. If you watch your machine, you will see the spindle turn on, rapid to z.1, then stop prior to tapping the hole. The control needs to do this to synch up the spindle and feed.

 

Someday, I am going to fix my post so it doesn't output the M3 when tapping. I haven't even checked if it is possible.

 

There is also a parameter to increase the tap retract speed, that you might want to play with.

 

Matt Wallace

Vertex Pharmaceuticals

[mcpgmr]

Question

 

We don't use rigid here but have used it many times at other jobs. G84 was standard tapping cycle and G84.1 was rigid and the feed had to be in IPR on one control in particular. What does the haas need to turn on rigid ?

[Guest]

There is a setting in the machine settings, once you turn it on you are rigid tapping

[Guest CNC Apps Guy 1]

M24 - Rigid Tapping (Synchonize) on a MORI SEIKI like I said in the post, "...modify for your situation..."

[DavidB]

James our Mori Seiki uses G841?

code:

---

 N25101 G21 G17 G40 G49 G80 G90

G64

M69

M79

G91 G28 Z0.

G91 G28 X0. Y0. A0. B0.

( #10-24 TAPRH TOOL - 251 DIA. OFF. - 0 LEN. - 0 DIA. - 4.826 )

M79

M69

T251 M6

G00 G54 G90 X0. Y0. A0. B0. S1407 M03

M78

M68

G43 H251 Z10.

G99 G841 Z-20. R10. F1489.5

G80

M09

M69

M79

G91 G28 Z0.

G91 G28 X0. Y0. A0 B0

M05

M30

%%

---

[Gary]

Hijack: What do you think of the mill (minimill) so far I would like to see one cut. Just would be for part time thing at home. Just Curious

[crazy^millman]

been covered many times do a search.

 

HTH

[Bob W.]

I looked long and hard at both the Mini Mill and a Fadal EMC. Ultimately I went with the Haas and I have absolutely no regrets. Looking back I thing buying a Fadal would have been a big mistake. I had some experience with a new Fadal 3016 ('04) and the Haas is much more rigid. Keep in mind that I am a bit of a novice, but I am really impressed with the Haas.

[Gary]

cool thanks what I was wondering about was compared to the emc

[Guest CNC Apps Guy 1]

quote:

---

...James our Mori Seiki uses G841...

---

 

What model???