O/T Rigid tapping lead mismatch

[Harryman]

I'm doing some rigid holder tapping (G84.2) with the Integrex. I changed the hole depth and got a lead mismatch. I can see that changing the R plane would cause that, but I'm surprized that changing depth would.

 

I'm pretty sure that it works in Mazatrol. Can you change depth on other rigid tapping machines and re-run?

[iowajim62]

Harryman,

 

You might check if the control has synchronous tapping support not just rigid tapping.

Our Mazaks have synchronous tapping that allows for restarts. On machines that don't have that capability you can't rerun taps.

HTH

[MACHINEMASTERG]

no problum on the haas with the rigid tap option in fact thats how we tap deep holes tap so deep then tap to final depth

[mayday]

should work, our Fanuc does a spindle orientate

at the R plane

[Harryman]

The options page on the control says Syncro. The EIA manual says so too.

 

Is there a parfrickin'rameter?

[iowajim62]

Hi Harryman,

Haven't read up on parameters yet but I did find in my EIA/ISO manual info about G63. Enters the NC unit into control mode suitable for tapping.

Don't know if that helps or not. G63 cancelled by G64 cutting mode. This is from FH-8800 Mill Manual so might not apply to Integrex.

Good Luck

[Harryman]

Thanks Jim.

 

No G63 listed. Tried it and got "Incorrect G code."

 

Checked depths; tap did not apparently slip.

 

Score: Harry=N Integrex=N+1

[crazy^millman]

Well are you tapping it in a normal plane or in an offset to normal plane. If you were tapping in say vertical ot horiztonal then you might not have a problem but if tapping on an angle it could be that it is only off a little in Z or a thing like that. I use to peck tap all the time on the VTc and never had any problems changing the depth or anything but maybe on a Intergrex with all the angles you might want to fix the ones not deep enough on the frist go around by hand. Do you have it going by feed per inch or feed per rev on the machine. It could be possilbe that is you were say feeding at 4 in a mintues on a 1" deep hole it is figuring the pitch from that so if the depth changes then you would need the feed to change alos just a crazy taught. Did it break off the tap. If not look and see that the tap didnt bottom out. I would also say anything over 1/2" on that machine I might think about thread milling I never liked rigiding tapping over 3/4" myself if it got that big millthread was the only way ot go on the VTC machine not the same machine but think alot more rigid than the intergrex is all.

 

Crazy Millman

[Jack Mitchell]

Harryman,

 

Please paste the lines of code and include the revised changes within a comment bracket.

 

I will imitate this on a fusion 640M tomorrow - VTC200C four axis.

 

Mazatrol restarts are a predictable breeze - I always unload the tool and allow the restart to load the tool itself (just good practice to eliminate possible mistakes).

 

Changing depth wont cause problems on the fusion - changing rpm will cause such problems.

 

 

Regards, Jack

[Thad]

Changing depth and retapping works fine here.

 

quote:

---

You might check if the control has

synchronous tapping support

not just rigid tapping.

---

This doesn't make sense to me. Isn't synchronous tapping just a description of what rigid tapping does?

 

Thad

[Harryman]

3/8-24, so light torque load.

 

Stopped way short of bottom.

 

S61 F.0417 feed in in/min. I just went with the posted values. Feed rate resolution .01 in/min.

 

Possible problem there, with feed rate. Should I calculate RPM from an obtainable feed rate say .05?

 

I'm sure that will seem turtle slow to you production guys. Material is 304L SST. 26.5" 0D X 1.25 thk. Don't dare break then back off.

 

No angle hocus pocus on this one.

 

M250

G0 B0.

M251

G17

G125 X0. Y0. Z0. R1 S0.

M212

G97 G0 C355.

G98

M211

M9

S61 M203

M248

G0 X7.655 Z.25

Y0.

G84.2 X7.655 Z-.4 R.2 F.0417

 

G98 is in/min...But .0417 is a feed/rev for 24 TPI.

 

Book says feed should be / rev.

 

[ 09-03-2003, 06:46 PM: Message edited by: Harryman ]

[crazy^millman]

Nope

quote:

---

You might check if the control has synchronous tapping support not just rigid tapping.

---

is the ability of a machine to line the tool back up to the same starting point everytime you restart it. edited(I am refering to oridienting the spindle to the same place everytime.) Just beacuse a machine can rigid tap does not mean you can retap a hole that you have tapped before.

 

Your code looks good but I alway put my Z to my R the same. Yeah one thing I always liked about the Mazaks' feed per rev you always knew what your feed per tooth was very quick.

 

That is the only thing I can see that might be giving you trouble starting at z.25 for the frist and if it peck tapping only coming back up to z.2 from there. Shouldn't do it but I always like to play it safe.

 

Crazy Millman

 

Yeah Jack have done that ohhhhh hate it when I broke taps off.

 

[ 09-03-2003, 10:51 PM: Message edited by: Millman^crazy ]

[Jack Mitchell]

Harryman,

 

Sorry I couldn't get to this today - too many alligators if you know what I mean.

 

Tomorrow for sure and this will be rather comprehensive.

 

Regards, Jack

[Harryman]

I hear you on the alligators Jack. I killed much of today trying to get the chip break peck drilling thing going. I tested it months ago and thought all was cool, (I goofed). Ended up rewriting the machine resident macro...Power off...Power on...Power off...Power on. And one more request to Dave for a post tweek. (Lurkers: please don't flame me on ease of chip break peck drilling. The Integrex doesn't do it the way you and I and the rest of the industrialized world think it should. )

 

That initial plane and R plane thing will be first on my testing list Millman.

 

Big plate, now with three helicoils and 29 hand finished holes, still in machine so I can't test the tapping thing.

 

I'll be watching the Forum tomorrow but I'll be on vacation next week. Hiking to the bottom of the Grand Canyon, and if all goes well, hiking back out too.

 

[ 09-04-2003, 06:29 PM: Message edited by: Harryman ]

[Jack Mitchell]

N005 G00 G90 G94 (Mazak Restart Test**1/4" thick - Free Cutting Brass**Mitchell**09/05/03)

N010 M06 T11 (#5 C-Drill T11/H11)

N015 G55 X0 Y0

N020 G43 H11 X-2.5 Y0 Z2.0 S2500 M03

N025 G99 G81 X-2.5 Y0 Z-.46 R.1 F13.1 M08

N030 X0

N035 X2.5

N045 G80 Z2.0 M09

N050 M06 T19 ("Q" Drill T19/H19)

N055 G43 H19 X-2.5 Y0 Z2.0 S2500 M03

N060 G99 G83 X-2.5 Y0 Z-.5 R.1 Q.1 F16.1 M08

N065 X0

N070 X2.5

N080 G80 Z2.0 M09

N085 M06 T12 (3/8-24 Machine Tap T12/H12)

N090 G43 H12 X-2.5 Y0 Z2.0 S1000 M03

N095 G99 G84 X-2.5 Y0 Z-.8 R.1 F.0416 M08

N100 X0

N105 X2.5

N115 G80 Z2.0 M09

N120 G91 G28 XYZ

N125 M02

%

 

Changed "Z" from -.8 to -.7 -.6 -.62 all were sync upon multiple restarts.

Changed "Z" from -.6 to -.8 did not sync upon restarts, despite inclusion and exclusion of H200 (assyncro/syncro in tapping cycle bumps rpm & feed to double upon exiting) (successive restarts at Z-.8 did sync)

 

On this machine/control the entry of F41.667 will error. You are indeed required to input the actual tap pitch. Therefore I conclude that the 640M fusion does indeed use the synchronous cycle when using G84.

 

Interesting point is that the control remained in G94 throughout and did not automatically perform a G95 as I expected - proven by going with G95 throughout this test as well while viewing the modal echo on the screen.

 

G84.2 was substituted as well as per the original query. I found no differences whatsoever between this or G84. there is mention of overriding bit 6 on Parameter F94 which stated to use this cycle to override synchronous tapping in the event that bit 6 is set to zero

 

Reducing rapid override to 25% and 50% also caused an over cutting occurrence in some restarts - this baffles me since it suggests a non sync condition.

 

Interesting point about the tool data screen is that if fixed is selected then the trust bump (returning feedrate) becomes valid. If floating is selected then the thrust bump is no longer available. This might well be a Mazatrol programming selection that remains outside the eia scope of things.

 

Peck tapping is available and totally - to die for- awesome - through Mazatrol; the finest feature is that feed hold will function on each peck exit if your concerned about reaching a “Z” axis stroke limit. I could not establish this in Eia programming and the manuals did not address this feature either. Perhaps somebody could copy and paste a reply to this thread so that I might attempt/attack this as well.

 

F91 00010000

F92 10100000

F93 00001000

F94 11010100

F95 01000101

F84 00100011

These are the parameters allowing full use of Mazak's auto tool measurement system when running with eia and Mastercam. (Mazak Renishaw S27R and MP12 probe) ultra serious stuff - if speed kills then I am already dying here.

Because of this feature there is no use for either G44 or G49 - this causes a "Z" downward motion IE: Crash

 

If G44 and or G49 are used within an eia program, then the tool data screen cannot have length values and the tool offset screen data must be used allowing for both "D" & "H" values on its screen. IE: I have used 1~16 for tool lengths & 17~32 for tool radii.

 

I have been doing this for a few years and believe the manual use of offsets to be redundant on Mazak/Mazatrol/Mitsubishi machine tools and controls - I still use this method on my VQC15/40 with the M32 control (I really should get around to changing these parameters some day).

 

 

Regards, Jack

[crazy^millman]

Man I miss those machines. Good follow up and explainantion Jack.

 

Crazy Millman

[PE @ IHS]

I would have to agree with Thad that rigid tapping and spindle synchronization go hand in hand. A machine cannot rigid tap if it can not do a spindle orient move (i.e. M19 on Fanuc). During rigid tapping, the tool needs to accurately synchronize spindle RPM with Z travel. The spindle orients within the tapping cycle for each hole. That's why the spindle stops temporarily before cutting each hole. If there was no spindle synchronization taking place, the spindle would keep on spinning at a constant RPM between holes.

 

Next time you rigid tap, press feed hold just before the spindle starts to feed into the hole. You will see that the spindle always points in the exact same direction for each hole, even if you a re-tapping the same hole.

 

 

On lathes, a similar concept applies. If you have rigid tapping, you automatically have spindle synchronization. Otherwise you have to use a floating holder to compensate for the lag in Z axis motion.

 

[ 09-07-2003, 10:02 AM: Message edited by: Peter Eigler ]

[Thad]

I've been meaning to get back to this one, but I haven't had the chance to collect any data.

 

Thad

[Jack Mitchell]

Peter,

 

M19 is not present between holes and it is not implimented immediately prior to the first tapped hole; the spindle stops as if it were an M05.

 

I went home and got fingernail polish from my wife and brought it in. (I can only hope that Harry doesn't see this on my bench before I'm done with this exercise)

 

I was also warned/scolded that the three colours that I selected were about $40 dollars worth - so I better not get them dirty.

 

I edited to 100rpm and swiped the passion pink on the collet at the "Y" negative quadrant between the first and second hole during tapping (feed hold between with a stopped spindle).

 

All restartes were accuarate to about 3~5 degrees, which in my opinion is not quite close enough for my liking. I am going to keep on this until I can come up with a syncronious solution via Eia, Mastercam, and Mazak.

 

Restarting in Mazatrol is effortless, I want to see this in Eia. I will also do the fingernail polish test in Mazatrol as well; heck I am even willing to buy some cool colours. - any suggestions out there from the California crowd?

 

I am so very sorry for saying that - I just dont know what's getiing into me lately.

 

Could somebody please paste a sample code for peck tapping in Eia?

 

 

Regards, Jack

[McRae]

Harry,

 

Did you contact National Applications? Those guys, know what you need and will answer quite quickly too. If you want the contact list that is an arm's length long, give me an offline message and we can get this sorted out.

[crazy^millman]

Hey Jack, By Calforina do you mean living here now and been living here. I will 100% agree with you on the whole EIA thing when it comes to Mazaks. I would always use my tool data from the Mazatrol side and set all of my parameter when doing so to support that. I find that part did very well and agree with the 3 to 5 degree variance you are getting also been there done that. I like i said earlier would always go back and hand tap holes if they were not to my liking when done the frist time. I never had any problems when doing peck tapping on the Mazaks in Mazatraol never even wanted to think about the fun it would be in EIA. I am refering to doing this on VTC's not Intregrex's Jack so understand 100% they are different but they also share soem of the same quirks as all machine do.

 

Crazy Millman

[McRae]

Harry,

 

Were there any diferences in the z-values between the passes??

 

Another thing is that if there is any pitch error that is unaccounted for and the tap didn't break - I would check to see if the tap may have pulled out of -or- pushed into the holder a little giving some axial error. Just some things that came to me in a dream...

[Harryman]

Good morning guys. Thanks for the research.

 

It's going to take some time for me to digest this all.

 

Had a super week off. They don't call it the "Grand Canyon" for nothing... Took me 7 hours to climb outa there.

 

Thanks Jack... Willing to walk into a machine shop with bottles of fingernail polish... You're a true friend.

[Harryman]

I finally got some time to analyze the replies. Thanks for all.

 

What's a "thrust bump"?

 

Integrex does not have any "F" parameters

 

G codes mentioned that do not apply to the Integrex:

G44

G49

G63

G94 (taper turning)???

G95 (exists as feed per rev in a G code series that I do not use)

 

T32 compatible G code series A uses G99 for feed per rev. My example code was using G98 (feed per minute) and I will alter that on next test. However, I suspect that G84.2 put the machine into feed per rev since a true feed rate of .0417/min would have just bored the hole with the tap.

 

There is no documentation for H to alter retract speed. There is P15 bit(0) "Overriding valid/ invalid of the return speed during synchronous tapping (parameter k70). K70 is set to 100. Looks like Mazak might allow changing retract speed... Just not in the program

 

Here's one just for fun: K75 "Selection about planetary tapping chip ejection" It's a Mazatrol parameter... Shucks! If I'm gonna tap planets I guess I'm stuck with Mazatrol, or planet chips.

 

R is incremental from the initial point where G84.2 was called. It shouldn't matter, but I'll get rid of R on next test.

 

E-mail coming your way Andrew. I don't think the tap moved...

[Ron Branch @ 5th Axis]

Well Harryman I dont know about the intregrex wit hthe paramters but I have played with me share of them on VTC and QT lathes. I think you are on the right path another trick I use to do when checking these problems was taking a indicator and checking that it stops in the same place everytime. I have found that if you adjust the parameters on the gain that it tweaks these little things. I have had problems with axis not lineing up properly when doing 4th axis stuff so if some of the aixs have these controls they might need ot be tweaked to make it run a little more precise. Might talk to the mazak guys about that and see what they think.

 

The Thrust bump is like a release of engery that bulids up in the spindle so even though for sake of topic you should go 1200 degree in rotation to tap the hole. Well the controller may tell the spindle to travel 1250 degrees to make it do the 1200 this would in essesnce create a excess travel for amount called but really only have traveled the distance wanted. When you back out of the hole this is like a release of the extra power need to get to that point. If the motor is powerful enough then this difference may only need to be 10 degrees to achieve this amount. This if you were to take a meter and look at the exact amount power at each point then it shows up really good like a chart. I only talk about the gain because from what I remember it had to do with the power being sent to the spefic places on each axis or spindle.

 

Well good luck I hope I have explained that correct.

 

Crazy Millman