rigid tapping - G94 or G95???

[BuxtonMachine]

I have been having problems rigid tapping (G84.1)on my Mighty mill w/A2100 contols. When reversing out of the hole the tap either breaks or is pulled out of the holder slowly. I realized that the Mastercam post for the A2100 was set to round my feeds off to 2 decimal places so I changed it to 4 decimal places and have corrected most of the problem.....but I am unsure if I should be tapping using a G94 or G95. I am still using Mastercam version 8.1 and the post is set to run G95 for all tapping (the post was written for Cincinnati machines). I've checked my owners manuals but they aren't clear as to why I should use a G94 or G95 in this case. Which would be better? Any help would be appreciated.

 

[PGW Steve]

Have you checked the math on the output code, are the spindle speed and feed correct for the tap pitch?? Does your machine support rigid tapping?

[DavidB]

Type "G95" on the line directly above the tapping cycle.

What that will do it will let you directly input the pitch in the tapping cycle and not have to worry about varing the pitch according to rpm. After the G80 at the end of the cycle do not forget to type "G94" to restore feed back.

 

eg

G95

G84 G98 S50 Z-?? R?? F=Pitch of Tap

G80

G94.

 

Also check your machine manual to see if a code is needed to Sync the spidle and feed rate.

My Fanucs need a M135 before the G84 line

[BuxtonMachine]

Yes I checked the math and it is now correct since the feeds are no longer being rounded off to 2 decimal places. Yes the machine does support rigid tapping.

The post used to take a feed of say F.0179 (56 pitch) and round it to F.02 when using a G95 code.

[BuxtonMachine]

DavidB

My post is already set to add the G95 before the tapping cyle and a G94 to return. So your opinion is that this works best? Why not just leave it in G94?

[DavidB]

G95 is feed per Revolution of the spindle.

 

I personely dont use G95 on a Mill for rigid tapping.

 

You want to retern the Machine back to G94 (Feed per Min/Inch) for milling ops.

 

HTH

[kinglouie V]

maybe an m29 before tapping line would help??

that's for fanuc though...

[mrainey]

Why would you want to use IPM for milling ops?

[Guest]

quote:

---

Why would you want to use IPM for milling ops?

---

Why would you not?

 

That's how the tools are sold, that's how the cutting descriptions are defined, ie Machinery's Handbook, all based on SFM.

 

There have been discussions in the past about tapping on a mill in IPR. Doing all the programming from a CAM system it makes zero sense to me.

 

I susbscribe to the KISS theory

 

Keep it simple stupid

 

[mrainey]

quote:

---

That's how the tools are sold,

---

All the cutting tools I've seen sold are described in term of IPR (drills, reamers, turning) or IPT (end mills, face mills).

 

IMHO, IPM is an additional calculation that doesn't accomplish anything useful.

[Guest]

As I have been fond of saying recently,

 

"different strokes"

 

In over 20 yrs, I have never seen a mill programmed in IPR mode but if it works for someone who am I to say different.

 

[Guest SAIPEM]

quote:

---

Why would you want to use IPM for milling ops?

---

Why?

 

Well for one, many of us began our careers actually cutting parts on manual machines.

 

MANY of the old manual machines had old mechanical dogs for feed settings and those were in IPM.

 

Try running an old Hydrotel.

 

You ask Why? I ask Why not?

 

While IPR can make things simple for a lot of people, (I love it for Mazatrol), IPM feed has it's advantages in plenty of situations.

 

If you can't find a useful reason for IPM feed then you haven't been machining or doing CNC long enough.

 

One right off the bat is for handling programmed spindle speeds that are higher than the maximum attainable by the machine.

I have three CNC mills that will gladly accept an S10000 M03 command even though the machines max out at 8K. They will also show the programmed RPM in the modal data.

These are all Fanuc controls.

The problem with IPR is that the feed will then be based on the modal RPM instead of the actual spindle speed. The downline problem becomes easy to see with very small end mills, they break.

[Guest SAIPEM]

quote:

---

I have been having problems rigid tapping (G84.1)on my Mighty mill w/A2100 contols. When reversing out of the hole the tap either breaks or is pulled out of the holder slowly. I realized that the Mastercam post for the A2100 was set to round my feeds off to 2 decimal places so I changed it to 4 decimal places and have corrected most of the problem.....but I am unsure if I should be tapping using a G94 or G95. I am still using Mastercam version 8.1 and the post is set to run G95 for all tapping (the post was written for Cincinnati machines). I've checked my owners manuals but they aren't clear as to why I should use a G94 or G95 in this case. Which would be better? Any help would be appreciated.

---

You're breaking taps because the spindle rotation and axis feed is out of sync.

 

G94 or G95 has absolutely ZERO effect on this problem.

 

You can compensate for this by using a compression holder even while rigid tapping.

[cadmonster66]

Buxton,

We have the same control at work, just a guess are you usig a "J" in your rigid tapping cycle, this tells how fast the tap comes out of the part "J2" will tell the tap come out of the part twice as fast as it went in, just a guess also when I right my tap cycle i use fraction feed rate

Example

1/20= F1/20

maybe this will help

John

Usually put the J right before the feed rate in my cycle

[mrainey]

quote:

---

If you can't find a useful reason for IPM feed then you haven't been machining or doing CNC long enough.

---

Thirty years. Feels like a long time.

 

 

quote:

---

One right off the bat is for handling programmed spindle speeds that are higher than the maximum attainable by the machine.

---

I try not to do that.

 

 

When I first started in CNC, the shop I worked at programmed machining centers in IPM and lathes in IPR. That's how I learned, never gave it a second thought.

 

I changed jobs and all the milling was in IPR. I asked why, and got this response:

 

Every tooling catalog lists feed recommendations in IPR or IPT. Why change your frame of reference?

 

If you see an IPM value in a program, you have no idea how hard the tool is working without factoring in the RPM so as to calculate IPR or IPT.

 

When optimizing at the machine in IPM mode, you can't play with the spindle override without also affecting chip load.

 

 

I thought about that for a few minutes, then bought into it 100% and never looked back.

 

As somebody said, "different strokes".

[Guest CNC Apps Guy 1]

IPR is my personal favorite.

[Guest SAIPEM]

For the most part it doesn't really make a difference, other than personal preference.

 

I do a lot of live-tooling programming on CNC lathes.

 

You won't find a Mazak Quick-Turn CNC lathe that allows live tooling to use IPR in G12.1 mode in EIA.

 

Everything has to be IPM for the live tool because of the C-Axis interpolation.

[Psychomill]

IPR is my favorite too. I'm at the opposite of John though,... in most of my years I've seen tap cycles programmed in IPR. Different strokes for different folks.....

 

Add to that, I'm also lazy. In IPR mode, when I change the RPM of the tap, I don't have to recalculate the feed since its constant....

 

[chowquoe^]

+1 Psycomill

 

I am lazy too, why change (2) when (1) works just fine, also I find that it is more operator friendly.

[Guest]

I don't want the operators changing sh*t

 

Everytime they do, I usually get screwed.

 

To me operator friendly is press the button and make the part, don't think about it, just do it.

[c-hook]

quote:

---

I have been having problems rigid tapping (G84.1)on my Mighty mill w/A2100 contols. When reversing out of the hole the tap either breaks or is pulled out of the holder slowly. I realized that the Mastercam post for the A2100 was set to round my feeds off to 2 decimal places so I changed it to 4 decimal places and have corrected most of the problem.....but I am unsure if I should be tapping using a G94 or G95. I am still using Mastercam version 8.1 and the post is set to run G95 for all tapping (the post was written for Cincinnati machines). I've checked my owners manuals but they aren't clear as to why I should use a G94 or G95 in this case. Which would be better? Any help would be appreciated.

 

---

Does your machine support rigid tapping? Some older machines (and newer ones too) require that you use a floating tap holder in order to compensate for the sync between the feed and spindle rotations.

[kinglouie V]

In almost 20 years I've used nothing but IPM for milling and IPR for the lathe. As for live tooling

IPM. I also started on manual equipment in Houston and can't remember anyone doing different down there. different strokes indeed.

[BuxtonMachine]

Yes the machine does support rigid tapping (G84.1), at least that's what the dealer ( worthless bunch of human beings) told me when I bought it. I put calls in to both Mighty ( the machine builder) and Siemens (A2100 controls) to confirm this, but as of yet have not heard back.

I have found that the only way I can rigid tap is if I use a floating tap holder, or I'll just keep breaking taps....however I'm one of those people that believe if your sold a product it should perform as advertised without needing a Rube Goldberg fix to get things going.

I did find that I prefer tapping in IPR , I can change the RPM without having to change the feed and the A2100 automatically does the recalculating for me.

[Randy Morton @ Clem Industrial]

John, are you saying that you higher monkeys to do the work? That's not very nice of you.

 

Maybe if you have a couple of extra's you can send them north to visit the great Canadian arctic I call home (Alberta).

 

BTW: No offense to any monkeys reading this

[Guest]

Got any banana's?