[DaveQueener]

Hi Gentlemen,

I've had a 1995 Milltronics Partner I with Centurion V controller for several years, but today was the first day that I tried to get the mill to tap a 4-40 hole using the G84 command. Basically, the mill center drilled and drilled the hole, but once it got to the tap holder, it simply dwelled over the hole about an inch above it and then began to barely feed towards it, maybe by a 1/10,000 every second while the spindle zipped along way too fast.

I spoke with a tech at Milltronics some months ago to find out if my mill was equipped with rigid tap--he seemd to think it was. So I am wondering if there is something wrong with my G code as BobCAD-CAM processes it. Here's a short sample program:

(Accucraft Coupler Pocket Fix)
(MACH_FILE=3AXVMILL.MCH)
(MTOOL T4 S1 D0.1875 H0.825 DIAM_OFFSET 4 = 0.09375)
(MTOOL T5 S1 D0.089 H5. DIAM_OFFSET 5 = 0.0445)
(MTOOL T6 S1 D0.112 H5. DIAM_OFFSET 6 = 0.056)
(SBOX X-0.185 Y-0.555 Z-0.12 L2.23178 W0.125 H0.38)
(END PREDATOR NC HEADER)
%
O100 (PROGRAM NUMBER)
(PROGRAM NAME - SR 36' TRUSSROD BOXCAR DRAFT BOX (ACCUCRAFT).NC)
(POST - CENTURION 5)
(DATE - SAT. 05/11/2013)
(TIME - 05:45PM)
N01 G00 G17 G20 G32 G40 G50 G69 G80 G90
(JOB 4 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP)
N02 T4 M06
N03 S1996 M03
N04 X0.25981 Y-0.21573
N05 G43 H4 Z0.88
N06 G81 X0.25981 Y-0.21573 Z0.111 R0.736 F7.9858 G98
N07 G80
N08 M05
(JOB 4 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP)
N09 T5 M06
N10 S7038 M03
N11 G00 X0.25981 Y-0.21573
N12 G43 H5 Z0.88
( *** MANUALLY EDIT V & D VALUES *** )
N13 G83 X0.25981 Y-0.21573 Z-0.21604 R0.736 V0.1 Q0.0445 D0.1 F7.0386 G98
N14 G80
N15 M05
(JOB 4 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP)
N16 T6 M06
N17 S3342 M03
N18 G00 X0.25981 Y-0.21573
N19 G43 H6 Z0.88
N20 G84 X0.25981 Y-0.21573 Z-0.14337 R0.736 B0. P0. F0.025 G98
N21 G80
N22 M05
(END OF PROGRAM)
N23 M02
%

Any ideas what may be wrong?

Thanks!

Dave Queener
Knoxville, Tennessee
(865) 280-2882

[TonyW]

Hi. We have a couple Milltronics using Centurion 6, one with rigid tap, one without. As far as I know, and verified at my machine, G84 is Milltronics 'soft' tap. G88 is the 'Hard' tap option. (Rigid tap). I've done tapping on the non-rigid tap machine, and just so happens I will be setting up rigid tapping on the other this week. I have modified the post processor to do it, just need to test it yet. Once I do I can post more for you. You may want to verify the G codes first to be sure. It is probably G88 for you too as that's what it seems Milltronics uses

[Machineit]

You may need to change your post so that it posts the G84 as a feed/minute rather than feed/revolution. I had to change it for my Haas.

N20 G84 X0.25981 Y-0.21573 Z-0.14337 R0.736 B0. P0. F0.025 G98

Your line about is feed per minute and it would take a long time to go Z-.14337 deep at feed of only 25 thousands per minute. (Actually about 6 minutes) I do not like the way cad systems figure tapping. Change your rpm to S1000 and your feed to F25.0 and I bet it taps just fine.

Mike

[Machineit]

In addition, if you want to write it yourself it is easy to figure. I tap most everything at 1000 rpm: so

1 divided by the threads per inch times 1000 equals your feedrate.

4-40 = 1/40 =.025 x 1000 = 25.0 feedrate

8-32 = 1/32 = .03125 x 1000 = 31.25 feedrate.

Makes it easy.

Mike

[jrmach]

""I tap most everything at 1000 rpm:""


Interesting.You are talking Aluminum ?
Out of curiosity,what would you tap a 1/2-13 one inch deep,,in aluminum ? ? Using a spiral Point Tap/thru hole.Speeds and feeds.I think I might be to slow on my speeds.

[TonyW]

You may need to change your post so that it posts the G84 as a feed/minute rather than feed/revolution. I had to change it for my Haas.

N20 G84 X0.25981 Y-0.21573 Z-0.14337 R0.736 B0. P0. F0.025 G98

Your line about is feed per minute and it would take a long time to go Z-.14337 deep at feed of only 25 thousands per minute. (Actually about 6 minutes) I do not like the way cad systems figure tapping. Change your rpm to S1000 and your feed to F25.0 and I bet it taps just fine.

Mike

Yes he is right. But only if you leave the G84 in place. If you change it to G88 (Milltronics Rigid Tapping Code), you will be trying to do 25 inches per rev

That's why I mentioned maybe verify the code with Milltronics first being that you're on a Centurion 5 and I'm on 6. Milltronics has many proprietary codes, so would be safer to check

[Machineit]

""I tap most everything at 1000 rpm:""


Interesting.You are talking Aluminum ?
Out of curiosity,what would you tap a 1/2-13 one inch deep,,in aluminum ? ? Using a spiral Point Tap/thru hole.Speeds and feeds.I think I might be to slow on my speeds.

I would probably use two or three passes so as to keep some coolant in the holes to prevent galling, but yep, I use 1000 rpm. Doing some 304 stainless right now and using 1000 rpm on an 8-32 tap.

For the most part, speed is power, if it has lubrication. Turning too slow weakens the tool. With enough speed, a straw can go through a tree in a tornado, but you would never be able to push it through slowly.

One Haas I used to run, had a chart from Haas on it with speed recommendations for tapping. Many of the speeds were from 3000 to 5000 rpm. I have an older machine and don't go that fast and you want to keep it slower for more accurate depth control. I would not want to tap a .200 deep hole to .190 deep at 5000 rpm!

Also remember to make your hole the correct size for your depth. For example, the basic drill and tap chart says the hole should be 27/64's or .422. But that holes size if for about 1/3 diameter of the tap for thickness or .166 deep. The correct size, from Machinery's Handbook, for a 1/2-13 tap 1 inch deep is .430 to .438 for class 1B and 2B and .4255 to .4313 for class 3B. Trying to tap 1/2-13 at the called for 27/64's or .422 is really tough on the tap as it goes to the full root of the tap and drags it down. Likely to seize or gall unless done very carefully.

For some interesting reading and an explanation of what I am saying, visit these two sites. The first one is a short explanation of the history of hole size for tapping and the second is a usable interactive guide to get proper holes sizes for tapping. A very good and handy site from OSG, the cutting tool and tap people.

Tap Drill Charts - The Right Information?

OSG Tap & Die, Inc.

Have fun! Mike

[jrmach]

""I would probably use two or three passes""


Now I am confused

Are you mixing 2 different methods of threading here ?

Thread Milling I understand 2 or 3 passes.Tapping,,2 or 3 passes,,you lost me.You mean 1/3 depth at a time,,to relieve chips and get coolant in ?

[Machineit]

Most rigid tapping machines synchronize the spindle at the same place for the start. So, on my Haas I can do multiple depth passes, like z-.5 then z-.75 and then z-1.0 and they are not crossed threaded.

G84 X0. Y0. Z-.5 R.1 F76.923
G84 X0. Y0. Z-.75 R.1 F76.923
G84 X0. Y0. Z-1.0 R.1 F76.923

Mike

[TonyW]

Hi Gentlemen,

I've had a 1995 Milltronics Partner I with Centurion V controller for several years, but today was the first day that I tried to get the mill to tap a 4-40 hole using the G84 command. Basically, the mill center drilled and drilled the hole, but once it got to the tap holder, it simply dwelled over the hole about an inch above it and then began to barely feed towards it, maybe by a 1/10,000 every second while the spindle zipped along way too fast.

Ok Dave,

I got Rigid tapping to work fine on Centurion 6. I had been adjusting my post to do it in the past just never got back to testing it. Worked great. Here's a sample of a tap drill and M6x1 tap hole. I needed to test the metric thread right away also:

(PROGRAM NAME - TAP TEST)
(POST - MILLTRONICS CENTURION 6)
(DATE - MON. 05/13/2013)
(TIME - 04:53PM)

N010 G00 G17 G40 G47 G49 G80 G20 G90

(FIRST CUT - FIRST TOOL)
(JOB 1 HOLE RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 .236 0.2360 Dia.118.0000 Deg. 1.2500 CL)
N015 T2 M06
N020 G90 G54 X0. Y0. S2500 M03
N025 G43 H2 D2 Z.1 M08
N030 G83 G99 X0. Y0. Z-1.05 R.1 Q.065 P0. F10.
N035 G80
N040 M09 M09 M05
N045 G00 G90 G32

(NEXT CUT - NEXT TOOL)
(JOB 2 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP)

(TOOL #3 .2362 M 6.0x1.0 1.0000 CL)
N050 T3 M06
N055 G90 G54 X0. Y0. S350 M03
N060 G43 H3 D3 Z.1 M08
N065 G88
N070 G88 G99 X0. Y0. Z-.75 R.1 F.0394
N075 G80
N080 M05 M09
N085 G32
N090 M02

(END OF FILE)
(END OF PROGRAM)

N095 M30
%

Have not quite figured out why I'm getting 2 G88 commands, but machine didn't mind it. I can upload my post processor if you want to give it a try. Just let me know

[jrmach]

Now I get you.Yup got the Haas VF2.I just do it in 1 pass.Interesting strategy for SS though,especially if blind hole.Anyhow,you answered my question,I am Dogging it.700 would usually be my choice.Doing onesy,twosy,,no real time loss though.However good to know.Those smaller taps scare me though.Hi-Jacking thread,I'll start new thread later,,more questions to come,if you don't mind?

[Machineit]

Now I get you.Yup got the Haas VF2.I just do it in 1 pass.Interesting strategy for SS though,especially if blind hole.Anyhow,you answered my question,I am Dogging it.700 would usually be my choice.Doing onesy,twosy,,no real time loss though.However good to know.Those smaller taps scare me though.Hi-Jacking thread,I'll start new thread later,,more questions to come,if you don't mind?

In case you don't get it started right away, before you repeat tap you have to have it enabled. Parameter 57, 5th line down is rigid tapping of course but line 7 is "Rept Rig Tap" and that must be enabled.

Mike

[DaveQueener]

Tony,

That's very kind of you--yes, I very much would like to see your modified post.

I'm still struggling with getting the right values for G88. I changed manually changed my G84 line of code to this:

(JOB 4 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP - 0.0890)
N16 T6 M06
N17 S100 M03
N18 G00 X0.25981 Y-0.21573
N19 G43 H6 Z0.88
N20 G88 X0.25981 Y-0.21573 Z-0.06837 R0.736 B2. P2. F2.50 G98
N21 G80
N22 M05

And wham! The spindle basically stopped rotating and tried to broach with the 4-40 tap. I had also added a two second dwell (the P value). Maybe I did not need this. And maybe I should have left F at 0.025--but it was doing the same thing--just super slowly feeding. So I did the division, and at a nice slow spindle RPM of 100 (I broke a tap yesterday when I tried to run the spindle at 1000 RPM and feed at 25), and came up with F2.5 Anyway, this did not work. Any ideas what's wrong with my code.

Oh yes, I do have an encoder on my spindle, so the machine is set up for rigid tapping.

Dave

Ok Dave,

I can upload my post processor if you want to give it a try. Just let me know

[TonyW]

Tony,

That's very kind of you--yes, I very much would like to see your modified post.

I'm still struggling with getting the right values for G88. I changed manually changed my G84 line of code to this:

(JOB 4 TAP RANDOM POINT PATTERN)
(FEATURE DRILL TAP - 0.0890)
N16 T6 M06
N17 S100 M03
N18 G00 X0.25981 Y-0.21573
N19 G43 H6 Z0.88
N20 G88 X0.25981 Y-0.21573 Z-0.06837 R0.736 B2. P2. F2.50 G98
N21 G80
N22 M05

And wham! The spindle basically stopped rotating and tried to broach with the 4-40 tap. I had also added a two second dwell (the P value). Maybe I did not need this. And maybe I should have left F at 0.025--but it was doing the same thing--just super slowly feeding. So I did the division, and at a nice slow spindle RPM of 100 (I broke a tap yesterday when I tried to run the spindle at 1000 RPM and feed at 25), and came up with F2.5 Anyway, this did not work. Any ideas what's wrong with my code.

Oh yes, I do have an encoder on my spindle, so the machine is set up for rigid tapping.

Dave

Ok. Couple things:

1- Don't use dwell if not needed. I never had luck with it. Remove the P code from program.
2- I have NO IDEA what a B code is. Try removing it.
3- You are missing a G99 (Return to rapid plane) in the G88 line. (G98 should be G99)
4- Your feed is output in inches per minute. Needs to be inches per rev. Right now you're trying to do 2.5 inches per rev, hence the broach action

Try my post, should give you a working sample. I've tested pretty much everything in it now and works well. Had to fix a few things, like the Machine Tool Compensation. It works now too. Also in your post, there's an option to turn on debug mode. Mine is at line#26 in post. Set it from debug_off to debug_on. It will then show you where the code is coming from in post. Give a try and let me know

[jrmach]

For a 4-40 tap at 100 rpm feed should be 2.5 ipm

at 1000 rpm feed should be 25 ipm

At least for my Haas,don't think it matters though.Is that right Tony/Mike ?

If it is just a couple of holes,I would hand tap that little sucker.Production is another story.

[TonyW]

Yeah JR. On my Haas its the same, it wants IPM for rigid tap. But on a Milltronics controller, it's in IPR. Easiest way to put is, on Milltronics:

G84 - Soft tap (Non-synchronous, Extension - retention holder) - Feed in Inches Per Minute
G88 - Hard tap (Synchronous Rigid Tapping) - Feed in Inches Per Revolution

There's a lot of 'different' codes on a Milltronics

[DaveQueener]

JRmach,

Right--if this were just a few holes, handtapping would be the way to go. But I am trying to get this issue sorted out so that I can cnc tap lots of little holes on my 1/20th scale brass steam locomotive frames. In fact, I just got a huge piece of aluminum today (14 x 48 x 2.5) to skim and then bolt to my mill's table so as to become a sacrificial table for milling these very sorts of frames from 1/4 x 2.5 x 36 slabs of brass. Admittedly the table may be a bit thick (but it was a gift), and what I do is model-making, specifically of F scale trains. I suppose I am one of the few guys who gets to live their dream--mine has been to produce large scale trains commercially. And I finally seem to be at the point of doing more than a few onesies and twosiees. You can check out some of my work here: Cumberland Model Engineering

Thanks again for all you all's help!

Dave

For a 4-40 tap . . . If it is just a couple of holes,I would hand tap that little sucker.Production is another story.

[jrmach]

Lots and lots of Brass it looks like.Is that what you tapping into ?Going to be some testing to get that just right.Get the right tap for sure.Right coating/style.Getting chips out the way is going to bey key,I imagine.