metric tap on haas

[PeterM]

Here's a nice tip for programmers with Haas milling machines. Our shop runs inch mode, but our customers sometimes want metric parts, go figure. Haas machine tools solid tap using exact FPM (three places F00.000)so take ANY metric tap, find the nearest multiple of 127 RPM to the recommended rpm and the feed is an exact fit. For example M8 x 1.25 , pitch = .049212598 x s508 = F25. or x s635 = F31.25 .Try that with any metric pitch, works great! Peter

[Charlie Pierson]

Thanks ,

 

cp

[jeff]

Why not just use a G95 and feed with IPR?

I use that for ALL of my taps.

Less room for calculating error,and it's easier to see that you have the correct feedrate no matter the rpm.

 

I also use IPR on some drills where I know the feed is correct but I want to tweak the Rpm's a little bit.

[Guest]

quote:

---

Less room for calculating error,and it's easier to see that you have the correct feedrate no matter the rpm

---

Yup, but if you set it once in your tool library, you'll never have to calculate it again.

[3rdstring]

quote:

---

Why not just use a G95 and feed with IPR?

I use that for ALL of my taps.

Less room for calculating error,and it's easier to see that you have the correct feedrate no matter the rpm.

---

+1

[Jeff the haas_guy]

jeff

 

G95 is a tapping mode? And what is

feed with IPR?

How would that be written?

[Guest]

haas_guy

 

To use the M8 x 1.25 from above

 

1.25/25.4 = .04921

 

So you'd have

T1 M6

G95

G00 G54 G90 X0. Y0. S550 M03

Height callout

G84 Z-.75 R.1 F.04921

 

and then to go back to IPM mode you have G94 at the end.

 

HTH

[Jeff the haas_guy]

Thanks jmparis

 

sounds easy enough to use all the time

when not programming with MC.

[mrainey]

I can't think of a single good reason to use IPM on a machining center if the control supports IPR. All published tool data is expressed as IPR. IPM, by itself, tells you nothing about how hard a tool is working.

[Chris Rizzo]

I'd say most tool data is expressed as FPT, or chip load. However even programming in IPR your only acheiving that value at engagements over 1/2 radial dia.

 

I hear what your saying though.

[jeff]

quote:

---

G95 is a tapping mode?

---

No, G95 is IPR mode,G94 is default mode for ipm feed.

 

Take the pitch of the thread, if it's M10x1.5, then the feed would be 1.5mm or F.059055 in G95 mode.

[mrainey]

quote:

---

I'd say most tool data is expressed as FPT, or chip load. However even programming in IPR your only acheiving that value at engagements over 1/2 radial dia.

---

Agreed, for milling tools.

[Guest]

In my neck of the woods, if you EVER were seen programming in IPR on a mill, you would be laughed out of the shop in fairly quick order.

 

Just not the way its done around these parts.

[Guest CNC Apps Guy 1]

I personally would like a switch or option to have feed rates expressed as IPR for Milling. When drilling it is very helpful.

 

I ALWAYS tap in IPR if the control supports it. Less rounding error and you can change the Speed without having to re-calculate feed.

 

JM2C

[chris m]

Nobody would laugh me out of anywhere, but 6'6" 265lbs counts for something....

 

Seriously, I programmed ALL G95 in the machines I have that support it before we got MC but now that I use Mastercam pretty much exclusively I have gotten lazy and just do RPM*IPR in the feed rate box and run G94 all of the time. Most of the guys who run milling machines are so used to seeing S1000 F3.0 that they get all flustered if the see F.003 instead. Seems simple to me but I have gotten a lot of bitching about it over the years and I just took the path of least resistance at the end. If you run proven feeds and speeds it doesn't matter a whole lot either way, in my opinion.

 

C

[Guest]

I hear ya chris, that's more what I was getting at.

 

Everyone is just used to seeing it one way and since the inmates DO run the asylum.....

 

Well, as you know that path of least resistance.

[PeterM]

Jeez, I go away for the weekend and look what happens. My tip is for a HAAS milling center, no g95 support there folks. I use G95 on machine tools that support it. I also have some older stuff cannot solid tap at all, so I note it in the set up sheet. Peter

[mrainey]

IPR is more logical and easier to work with for on-the-floor optimizing.

 

The parts come out the same either way.

 

If you've been using IPM for years and that's all the shop people have ever seen, you'd better leave it alone.