Style of tap ?

[Scott Bond]

Hi all What style of tap are you guys using for peck tapping?

 

Today I am spiral tapping 6-32 holes .450 deep(.100 pecks)it taps good the first hole, then breaks on the second.

 

two flute?

spiral?

 

I need some tips

[G Caputo]

Scott,

 

I could be wrong here but I don't think spiral taps are for pecking, just 1 shot to depth. We use osg taps with the elektralube coating and we have very few problems with breakage.

 

Greg

[Tony]

Scott,

I have used 3 Flute spiral

"NC" Style down to 1/4-20

 

#500

I have now become one with the Software

 

[ 08-06-2003, 05:46 PM: Message edited by: Tony ]

[MACHINEMASTERG]

does mastercam support peck tapping ???if so how

[Slixmix]

What material?

[G Caputo]

My most logical guess would be that it would have to be supported by your post. One of our machines has the cycle in the machine (cycle definition 209) and the cyle we use is 17 which is fairly close. You could probably modify the post with a custom cycle and away you'd go. Just my best stab in the dark though.

 

Greg

 

45 minutes to $1 beer nite

[crazy^millman]

Well are you doign a thru or a blind. I would think blind but just wondering. If you are doing very hard material look at the EXO-TAP it works greta in harden material up to 55-rc. I also use alot of HY-PRO taps both are made by OSG. If you are doing a blind hole and are worried about getting enough thread I would use a modified bottom sprial flute tap and do it in one shot. It give you chip evuaction and gives u good thread to the bottom of your hole. Good Luck

 

Crazy Millman

[CAM-mando]

quote:

---

What material?

---

+1

[Jack Mitchell]

+ All of it.

 

HyPro spiral point is best - bottoming is not very strong.

 

I usually peck at 1.5~2 threads depending on material type, I believe Chris mentioned just do it straight up with G84 rather than peck tapping.

 

If you come back to us with a response please state the material and what rpm was used prior to the question - every little bit helps.

 

Regards, Jack

[Scott Bond]

Plus one --Aluminum

Please excuse my slow responce,,, and now I will be gone untill later tonight.

Thanks for your replies, I will have more tommorow.

 

It's my 18th AA birthday

[tsewyek]

Scott,

 

Sincere Congrats on your 18th. My wife's about to do her 16th. in Sept. I know what a cliche it can sound like but one day at a time!

[Chris Rizzo]

If your using spiral taps and peck tapping/chip breaking, your probably getting the chip all jammed up in the flutes, thus causing the breakage. Spiral fluted taps pull one long nice continous chip out through the flutes. They are rather "weak" taps from the reduced cross section, and don't take kindly to reverse/foward torque changes. That said, just run em' in one time and you'll be suprised that they do work.

We run about 500 holes in 6061 wrought plate before changing a 6-32 tap. It may go a few hundred more holes for all I know, but I'd rather change the tap than scrap a part...Keep the coolant flowing too.

[CAM-mando]

I have not had the need to peck tap aluminum, but cant say I have any recent memtory of 6D holes either. Most of the peck tapping I have done has been as a last resort in Titanium down to 0-80 3X Deep or so. In our abblications, we were able to use spiral point gun taps with out the need to bottom tap.

 

Even though the spindle is synchronized, we generally have been using Tension Compression Style Holders.

 

I tend to lean towards CMR's thinking about the spiral tap (Im assuming we are talking RH Cut / RH Spiral).

 

My peck cycle in MC is set up to use initial depth which I go as deep as I can safeley, then subsequent pecks which I normally keep around 2P.

 

In deep tapping (3D+) with small taps (<#8) I run slower than the handbook speed.

 

[ 08-06-2003, 11:31 PM: Message edited by: CAMmando ]

[Quickmike]

Try using a forming tap. No chips, strong body with no flutes to reduce breakage. I have used Balax brand before and had good luck in aluminum. Hole size does become critical though. This is because the metal is moved to form a thread and depending on how much mat'l is left this will directly reflect in the % of thread. I usually throw a healthy chamfer around the hole before forming because it tends to raise the material up in the localized area around the hole. Maybe like a .04 x 45 degrees. For a 6-32 drill size is .124,.125,.126. These sizes are supposed to result in 75%,65%,55% respactively. HTH

[Guest CNC Apps Guy 1]

quote:

---

...does mastercam support peck tapping ???if so how...

---

Yes and you need to make some post modifications.

 

I think you may be pecking too deep also. As a general rule, I peck around 100% of the Maj. Dia. true it's more pecks but I like to keep things cleared out as much as possible.

 

JM2C

[Lathe-Mill]

have you try roll form taps?...

[Kenneth Potter]

Roll taps man....use ROLL TAPs!!......I use Standard cut taps only a s a last resort.

I also love those thread monster solid carbide(powederd) cut taps...250 to 300$ a piece....there kick AR@#!

interpolate a rough & finish pass for each hole .......last forever!!!!

 

I make it.... you sell it !

[A-ron1286490684]

+10 on the EXO taps, they are almost bullet proof. And for roll taps the 6-32 is probably the BEST candidate since it's minor vs. major percentage is the worst.

 

If I'm not mistaken some machines require a parameter or callout on the G84 line specifically for peck tapping. I think we used to do that long ago in the old Haas VF3 and had good results but I don't remember which it was. If I was celebrating ANY kind of AA aniversary myself I'd probably be able to pull that out of the pickle jar for you.

 

EDIT: Congratulations Mr. Bond!

 

[ 08-07-2003, 03:09 PM: Message edited by: A-ron ]

[Scott Bond]

Hi everybody

Thanks for the coaching, I will

be trying several of the choices.

My main problem seams to be picking .100 deep, and it will be changed to .030 deep, and I will change to form-taps.

 

Nice to hear from you Potter

[MetalMarvels]

I am a little late on this thread, but form taps in 6061 are definitely the way to go. Also +1 to Quickmike - they do throw up a healthy "burr" going in. I usually run a fast chamfer on the larger tapped holes and a small countersink on the smaller tapped holes to give a "nice" entry.

 

 

ps - I typically only get the bottoming taps and have had no problems with running 6-32 taps in as far as .75 deep in one pass. I also change mine out at about 500 holes - it really bites to have a tap break on the last op after an hours or two of work.

 

[ 08-07-2003, 03:55 PM: Message edited by: MetalMarvels ]

[Chris Rizzo]

There was a discussion a little while back that got into forming taps...just watch out for using them on the cast alum. tooling plate.

previous form tap topic