Peck Tapping on a Mori Horitontal NH6300

[Cad-Camr]

I would like to initiate a peck tapping cycle on our Mori. We doing some fairly deep 5/16-18 holes.

We are using a good OSG Thru Coolant Low Spiral Tap. In my past experience you could add a Q value and it would work. Not with this control. Any help is much appreciated.

[cincy k]

What control is it?

[Cad-Camr]

The front of the control says MSX 501 III. Much newer than anything Ive ran before.

[HEED]

Have you thought about thread milling? Tapping is good if you just have a few holes, but thread milling will produce more consistent, and better quality threads than a tap can. I don't know for sure on the Mori control, but on the Mazak, you just add a Q to the G84 line.

 

EDIT~ oops I didn't see in your post that you knew about the Q thing. I don't know. Some controls dont support the peck cycle. Some controls if you have a rigid tap setup (the tap orients before each hole is tapped) you can simply program a different depth for each time you go around the set of holes. But I don't think the tap will track to go in the same hole unless you have the rigid tap feature.

[Guest CNC Apps Guy 1]

That may be a Mitsubixxxx control and unable to do that.

[Rob @ Target Machine]

Try adding progressive Z depths to the cycle like this:

 

G98 G84 Z-.1 R.05 F.0556

Z-.2

Z-.3

Z-.4

G80

 

If that works for you, I have a peck tapping cycle that I can set you up with.

 

 

Let me know how it goes.

 

 

FYI Guys - You can peck tap in any machine that has rigid or solid tapping.

 

Even if you have to call the cycle over and over

like:

 

G98 G84 Z-.1 R.05 F.0556

G98 G84 Z-.2 R.05 F.0556

G98 G84 Z-.3 R.05 F.0556

G98 G84 Z-.4 R.05 F.0556

G80

 

 

Joking aside, I'd rather thread mill any day of the week.

[latheman]

depending on the material i would try a form tap with a reduced shank. we thread mill 1 1/2-12 so im not familiar with anything smaller. is thread milling not a slow process and the chips still build up at the bottom of a deep hole. just curious

[latheman]

btw no peck needed (form taps)

[Cad-Camr]

Good Morning All, Thanks for the replies I am programming the deeper tapped holes with progressive Z depths and that works fine. I guess I was looking for an easier way out. This is a high end cell system with rigrd tapping and I would think It would support peck tapping. The control is similar to Fanuc but may be customized by Mori Seiki. I just started getting involved in the programming end after being away from it for 5 years. (Last shop didnt have horizontals). Ive got some catching up to do. Thread milling is awsome in a lot of Apps but some holes are 3" deep and the additional tooling gets denied$. Thanks for the suggestions. If I get this resolved I'll post the solution. Thanks again

[JMWorks]

Been a while but I used to run a NH6300DCG and I believe peck tap was a seperate G-Code and may have even been an option. Could be wrong, like I said it has been a while and we always used the form taps so peck tapping was never used if it had but I think I recall seeing that in the programming manual.

[Craig-B]

Try this

(Example 1)

G98G84.2X0.Y0.Z-2.25R.1Q.75F10.

G0G80Z1.

 

(Example 2)

M29S2500(spindle speed)

G98G84X0.Y0.Z-2.25R.1Q.75F10.

G0G80Z1.

[Cad-Camr]

Okay! Right about now I'm feeling pretty stupid. It seems the post doesnt support peck tapping. Previously I manualy edited in the Q value and got an alarm. So I started researching expecting to find a different command such as G84. something or an alternate adress for Q such as K. After Craigs reply I tried it again and the Q worked. Sorry for the wasted effort. Thanks for your support.

[Mic6]

Where's the bow machining videos?

[Cad-Camr]

Thats confidential. (I Think) We wouldnt want that to get to Matthews or PSE or Hoyt, Martin, Bear etc.(FYI Not Rocket Science). By the way Mic I used to work in your area. Armstrong Technology, Calmax Technology, A&D precision. 20 years in the Bay Area.

[lwells]

I'm running the same machine with a mx701III. Latest and greatest. Control is a fanuc. I'm using the mpmaster post. In the tool paremeter page i can select tap and I get a peck option. Select peck depth and post. Outputs a g94 then m29 s200 and puts a q value in the command line. Make sure you have the m29 s0000 before the g84.

[Cad-Camr]

What version of mcam are you runing? Im running X2 MR2 and I dont get the peck option

[Rob @ Target Machine]

Cad-Camr - If your machine is peck tapping with the Q value you might be interested in how to

add the "peck" box and get the Q to output on your tapping lines.

 

Add this to your ptap postblock: "[if peck1$, *peck1$]".

 

You will get a Q output (if it isn't zero) from the value you put into 1st peck box on the tapping dialog box.

 

This is from the X4 Mpmaster Post.

 

code:

---

ptap$            #Canned Tap Cycle

pdrlcommonb

#RH/LH based on spindle direction

if rigid_tap, pbld, n$, *sm29, *speed, e$ #Rigid Tapping

if use_pitch = 0,

[

pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout, pindexdrl,

prdrlout, [if peck1$, *peck1$], *feed, strcantext, e$ # <---------------Here

]

else,

[

if metvals, pitch = n_tap_thds$ # Tap pitch (mm per thread)

else, pitch = 1/n_tap_thds$ # Tap pitch (inches per thread)

pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout, pindexdrl,

prdrlout, [if peck1$, *peck1$], *pitch, !feed, strcantext, e$ # <-------Here

]

pcom_movea

---

Then in your control def you can change "1st Peck" (which is probably greyed out), to 'Peck", so you can enter a number in the box. Assuming that it is disabled in your post/cd (it's disabled by default).

 

 

 

 

Then your tapping dialog should look like this.

 

 

 

 

 

HTH

 

[ 08-14-2009, 08:54 AM: Message edited by: Mastercam Guru ]

[Mick]

I believe there is a parameter value to switch between incremental withdrawal, and full withdrawal, when peck tapping. I'm not certain what it is.

 

We use peck tapping on our Okuma. It has two seperate G codes to call the peck tapping, and it works great.

[Guest CNC Apps Guy 1]

Yes there is a parameter that dictates "High Speed Peck" style or Full Retract.

 

#5106.6 = 1 "Q" while Rigid Tapping is Valid

 

#5200;

 

- Bit 0 - G84 Method for specifying rigid tapping

0 : An M code specifying the rigid tapping mode is specified prior to the

issue of the G84 (or G74) command. (See parameter No.5210).

1 : An M code specifying the rigid tapping mode is not used. (G84

cannot be used as a G code for the tapping cycle; G74 cannot be used

for the reverse tapping cycle.)

 

Bit 1 - VGR Any gear ratio between spindle and position coder in rigid tapping

0 : Not used (The gear ratio is set in parameter No.3706.)

1 : Used (The gear ratio is set by parameters Nos. 5221 through 5224 and

5231 through 5234.)

NOTE

For serial spindles, set this parameter to 0 when using the

DMR function for position coder signals on the spindle side.

 

Bit 2 - CRG Rigid mode when a rigid mode cancel command is specified (G80, G01

group G code, reset, etc.)

0 : Canceled after rigid tapping signal RGTAP is set to “0”.

1 : Canceled before rigid tapping signal RGTAP is set to “0”.

 

Bit 3 - SIG When gears are changed for rigid tapping, the use of SIND

G033> is

0 : Not permitted.

1 : Permitted.

 

Bit 4 - DOV Override during extraction in rigid tapping

0 : Invalidated

1 : Validated (The override value is set in parameter No.5211.)

 

Bit 5 - PCP Rigid tapping

0 : Used as a high–speed peck tapping cycle

1 : Not used as a high–speed peck tapping cycle

 

Bit 6 - FHD Feed hold and single block in rigid tapping

0 : Invalidated

1 : Validated

 

Bit 7 - SRS To select a spindle used for rigid tapping in multi–spindle control:

0 : The spindle selection signals SWS1 and SWS2 (bits 0 and 1 of G027)

are used. (These signals are used also for multi–spindle control.)

1 : The rigid tapping spindle selection signals RGTSP1 and RGTSP2

(bits 4 and 5 of G061) are used. (These signals are provided expressly

for rigid tapping.)

 

HTH