MPFAN mod for tapping question

[chris m]

Hello

 

Does anyone have a post for a 1995 Matsuura RA2 with pallet changer and Yasnac MX3 control?

 

But seriously,

 

I'm trying to get the post to output code like this for tapping cycles:

 

(TOOL 3 1/4-20 HELICOIL TAP)

(TAP 12X)

N125 G00 G17 G40 G80 G90 G98 G94

N130 T3 M6

N135 M42 S180

N140 G56 J4 X1.3535 Y-2.3443 T4 M3

N145 G43 H3 Z.1 M08

N150 G93

N155 G84 Z-1.153 R-.294 F.050 S180

.

.

.

N165 G94

N170 G80

N175 M09

N180 M05

N185 G53 Z0. M19

N190 M01

 

because the machine needs line N135 [even though the book says it doesn't, it won't run without it] as a preparatory command and I can't get it to work because the 'drillcyc' value [which is '3' for tapping] doesn't seem to get updated until long after where I need to use it.

 

Any ideas on how I can get this to work?

 

Oh yeah, using MPFAN off the CD, modified for my needs

 

Thanks in advance

 

C

 

[ 09-29-2003, 12:39 PM: Message edited by: chris m ]

[gms1]

I have never used a Yasnac control. Im strictly a Fanuc guy, but that N135 line appears to be a Rigid Tap cycle.

If that is the case, you could try what I did to my fanuc post. I use a miscellaneous integer to add my rigid call out (fanuc control is M29) and spindle speed before the canned cycle. I also use a miscellaneous real to turn off the spindle speed call out on the first line of my canned cycle. Since my fanuc post spits out speed and spindle direction in the beginning of a cycle.

 

Greg

[J Coulston]

ptap #Canned Tap Cycle

pdrlcommonb

#RH/LH based on spindle direction

if use_pitch, pbld, n, "G95", e

if use_pitch = 0,

[

pcan1, pbld, n, "M29", *speed, e #********Added 12/17/02/*******

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

prdrlout, *feed, strcantext, e

]

 

Outputs

N6874 G54.1 P10 M08

N6875 G00 G90 B0 X1.4003 Y-13.9289 S1500 M03

N6876 G43 H17 Z1.25 T7

N6877 M29 S1500

N6878 G98 G84 Z.115 R.4952 F46.88

N6879 Y-9.8939

 

Does the M42 have to come before the workoffset or just before the G84?

 

The code above runs on Fanuc OM and 16i.

 

John

[chris m]

John, my post for my Millac 438 with a Fanuc 18 is setup basically the same way as yours, though without the spindle speed. This is not what I need for the Yasnac. The code has to be exactly as shown in my example.

 

Greg

 

if you modify your ptap sub in your post to look like Johns or like this:

 

ptap #Canned Tap Cycle

pdrlcommonb

result = newfs(12, feed) # Set for tapping Feedrate format

pbld, n, "M29", e #(cdm)

pcan1, pbld, n, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *feed, strcantext, e

pcom_movea

 

You won't need that misc integer for tapping M29 output

 

Similarly, I do not wish to use this type of thing to get my output the way I want.

 

I don't really understand what you're saying about the forced spindle and rpm output but you should find *speed and *spindle on whatever postline is causing this; just remove the asterisks and the code should look like what you want.

 

C

 

Thanks for the suggestions, guys, keep 'em coming.

 

[ 09-29-2003, 10:26 AM: Message edited by: chris m ]

[Guest]

Chris:

 

How about checking for tool_typ. Right hand tap is 4 and left hand tap is 5.

 

Try this line:

 

if tool_typ > 3 & tool_typ < 6, "M42", "S180", e

 

 

HTH

[fboike]

Chris

what if you add an if or else statment in

pdrlcommonb that should put the code where you need it.

[chris m]

Marc-

 

I'll try that, thanks

 

fboike-

 

The post doesn't get to pdrillcommonb until too late to post the code where I want it. I actually moved the pdrillcommonb call up to where I wanted the code to post and it still didn't work; it doesn't seem like the NCI file makes the data available until too late. I was thinking I could buffer the whole tool worth of code before posting but I don't know how to do it.

 

C

[McRae]

Chris,

 

Is this a gear change or something that the control thinks of as a gear change??

 

If multiple gears are not available then I would suggest that you investigate the machine parameters and correct the issue that way.

 

Only offering potential solutions...

[McRae]

I have read the other responses to this question and have a thousand more of my own but have distilled down some to the ones below...

 

1)Is the M42 required on the same line as the spindle speed or can it be anywhere before the actual tapping call. I remember that the M29 from the Enshu with a Fanuc control would slave the z-axis to the spindle encoder feedback for the rigid tapping cycle.

 

2)Are you trying to rigid tap or is this specifically for every tapping call.

 

3)Do you have the use of the Misc Integers avail in your post?

 

4)Does your code have to finish with the G49 inside of the code before the G80?

 

5)That gear thing is still bugging me...

 

 

One post way would be to create a set of logic during the spindle command that would look at a Misc Integer and then hard codfe in a M42 S***

 

 

Hope we gave you some more options here...

[chris m]

Marc you are the MAN!

 

This works beautifully:

 

if tool_typ > 3 & tool_typ < 6, pbld, n, "M42", *speed, e # Output for tapping

 

I'll try to break it but so far seems pretty bulletproof. Thanks a lot, I wouldn't have thought of that [though next time I will].

 

Andrew, thanks for the laundry list I have to answer

 

First of all, M42 is high range for the gearbox which can be commanded for tapping even if the RPM is out of the high-gear range [don't ask me why as I didn't build the freaking thing]

 

Next:

 

 

1]Is the M42 required on the same line as the spindle speed or can it be anywhere before the actual tapping call. I remember that the M29 from the Enshu with a Fanuc control would slave the z-axis to the spindle encoder feedback for the rigid tapping cycle.

 

- Code must be exactly as in my sample

 

2]Are you trying to rigid tap or is this specifically for every tapping call.

 

- Machine does not have the rigid tap option, this must be in every tap call

 

3]Do you have the use of the Misc Integers avail in your post?

 

- Yes, but it would be a workaround I'd rather not use until all other options are exhausted

 

4]Does your code have to finish with the G49 inside of the code before the G80?

 

- I need the G94 before G80 but that is already all set as I can use the if drillcyc = 3 argument at that point

 

5]That gear thing is still bugging me...

 

- Me too, but we have 1000 programs like that already so I'm just rolling with it

 

 

Thanks to all of you guys

 

C

[McRae]

quote:

---

Marc you are the MAN!

 

This works beautifully:

---

Sure, until you have to tap left handed holes...

 

Thanks for humouring me. I think the more elegant solution (though I'm not the one doing the work or footing the bill!) is to use the misc int or to delay the posting as you have suggested.

[chris m]

quote:

---

Sure, until you have to tap left handed holes...

---

Actually, not, as Marc's way is checking tool types for both LH and RH taps

 

Don't like the mi option because if you forget to turn it on the program bombs in the machine

 

The buffering option I'd still entertain..

 

C

[Roger Martin from CNC Software]

Load up the MPFAEDAL2.PST that is on the CD

 

Search for "tap_speed" to see the areas that

setup the Rigid Tap mode prior to the cycle.

[gms1]

Chris m:

 

Yes I did start working on my post to set it up for that type of easy output. Problem is, some of our controls do not have rigid tapping cycles. And since I am not the only one who uses this post I had to set it up as a toggle switch to use it when I could.

Just thought it would be a quickie fix for it. But seems you got the cherry answer

 

Greg

[chris m]

Roger

 

Thanks, I'll look at it.

 

Greg

 

Just wanted to give you options; sometimes you don't see all the angles when you first look at something. I use 'machine codes' in some posts where we have more than one machine with the same post so I just set miX to '1' for a certain machine, '2' for another and have all of the machine-specific coding in the post with if statements.

 

I also have a couple of posts for the same control with different names if the 'code' crap is too much different.

 

Just some ideas

 

This forum rocks

 

C

 

[ 09-29-2003, 03:10 PM: Message edited by: chris m ]

[McRae]

quote:

---

I also have a couple of posts for the same control with different names if the 'code' crap is too much different.

 

Just some ideas

---

Brute Force will overcaome all obstacles...

[gms1]

quote:

---

Greg

 

Just wanted to give you options; sometimes you don't see all the angles when you first look at something. I use 'machine codes' in some posts where we have more than one machine with the same post so I just set miX to '1' for a certain machine, '2' for another and have all of the machine-specific coding in the post with if statements.

 

I also have a couple of posts for the same control with different names if the 'code' crap is too much different.

 

Just some ideas

 

This forum rocks

---

Hmmm this sounds good.....

 

 

Greg