Problems with Solid/Rigid tapping

AMVERGINO · Aug 1, 2019

Hello,

I just joined PM and I was hoping to get a little help with Solid/Rigid tapping issue I'm having.
The Machine I'm using is a Kitamura MyCenter3x with a yasnac I80M controller I'm still just using HSM Express that I downloaded for free and is baked into my Solidworks.

My question is I have been trying to thread some aluminum parts using the solid tapping function and cannot get it to produce anything worthwhile. One weird thing is that HSM outputs a spindle speed at the beginning of the operation and then again in the G84 line of code. No matter what either one is set at before the tap goes into the part and while its initializing the spindle stops then begins to rotate very slowly while its descending into the part. I've deleted the Speed command in the G84 line and the same thing happens. I'm not quite sure what's going on or what if anything I'm doing wrong. Any help would be greatly appreciated. I'm attaching just a small example of the code I'm running for a tap cycle with a M10 x 1.5 hole. It looks like its working perfectly in the air but obviously something is off. I know that my spindle speed is too slow right now in the code below I'm just trying to keep it at something I can watch.
Thanks!

O00054 (M10 TAPPED HOLE)
(T0014 D=0.3937 CR=0. - ZMIN=-0.625 - RIGHT HAND TAP)
N10 G90 G94 G17
N15 G20
N20 G28 G91 Z0.
N25 G90
(DRILL3)
N30 M09
N35 T14
N37 M06
N40 S381 M03
N45 M08
N55 G00 G54 X1.875 Y-0.75
N60 G43 Z0.6 H14
N70 G00 Z0.2
N75 M03
N80 G93
N85 G98 G84 X1.875 Y-0.75 Z-0.625 R0.1655 F0.0591 S381
N90 G80
N95 G94
N100 Z0.6
N110 M09
N115 G28 G91 Z0.
N120 G28 X0. Y0.
N122 M05
N123 T20
N124 M06
N125 M30

Larry Dickman · Aug 1, 2019

Don't know much about yaznak, but on a fanuc you need to start the spindle with an M29 S*** command. It's been a while, but I seem to recall the same results without it

Delw · Aug 1, 2019

AMVERGINO said:
Hello,

I just joined PM and I was hoping to get a little help with Solid/Rigid tapping issue I'm having.
The Machine I'm using is a Kitamura MyCenter3x with a yasnac I80M controller I'm still just using HSM Express that I downloaded for free and is baked into my Solidworks.

My question is I have been trying to thread some aluminum parts using the solid tapping function and cannot get it to produce anything worthwhile. One weird thing is that HSM outputs a spindle speed at the beginning of the operation and then again in the G84 line of code. No matter what either one is set at before the tap goes into the part and while its initializing the spindle stops then begins to rotate very slowly while its descending into the part. I've deleted the Speed command in the G84 line and the same thing happens. I'm not quite sure what's going on or what if anything I'm doing wrong. Any help would be greatly appreciated. I'm attaching just a small example of the code I'm running for a tap cycle with a M10 x 1.5 hole. It looks like its working perfectly in the air but obviously something is off. I know that my spindle speed is too slow right now in the code below I'm just trying to keep it at something I can watch.
Thanks!

O00054 (M10 TAPPED HOLE)
(T0014 D=0.3937 CR=0. - ZMIN=-0.625 - RIGHT HAND TAP)
N10 G90 G94 G17
N15 G20
N20 G28 G91 Z0.
N25 G90
(DRILL3)
N30 M09
N35 T14( M06 and T14 should be on same page)
N37 M06
N40 S381 M03 its not needed as you have it below in the g84 line
N45 M08
N55 G00 G54 X1.875 Y-0.75
N60 G43 Z0.6 H14
N70 G00 Z0.2
N75 M03(you dont need this )
N80 G93
N85 G98 G84 X1.875 Y-0.75 Z-0.625 R0.1655 F0.0591 S381 your R should be .200 to match the "z" in line n70 (not required)
N90 G80
N95 G94
N100 Z0.6
N110 M09
N115 G28 G91 Z0.
N120 G28 X0. Y0.
N122 M05
N123 T20
N124 M06
N125 M30

its going to go slow cause your only going 381 rpm

AMVERGINO · Aug 1, 2019

Thanks for the reply, The Spindle is getting commanded in two places in the code on the yasnac its M03 S... and that's being commanded at the beginning. My problem is that it turns on at the speed commanded but once it enters the canned cycle it drops dramatically. Neither the speed at the beginning or the one in the G84 line make any difference. My guess is its around 100RPM maybe slower when its actually doing the tap cycle

AMVERGINO · Aug 1, 2019

Thanks for the reply but its dropping to maybe 100 rpm the 381 is just a speed I put in so I can watch it. Like I explained above the spindle drops to a crawl as soon as it enters the G84 Canned cycle. I could have it set at 3000 rpm but as soon as it enters G84 it comes to a crawl

JCarroll · Aug 1, 2019

AMVERGINO said:
Thanks for the reply but its dropping to maybe 100 rpm the 381 is just a speed I put in so I can watch it. Like I explained above the spindle drops to a crawl as soon as it enters the G84 Canned cycle. I could have it set at 3000 rpm but as soon as it enters G84 it comes to a crawl

This works on the one I ran.
Same machine and control.

N1 G0 G90 G40 G80 G17
N2 G91 G28 Z0.
N3 T32
N4 M6(M11 X 1 TAP)
N5 M3 S500
N6 G90
N7 G60
N8 G0 G54 X-4.5638 Y-3.739
N9 G43 Z0.375 H32 M8
N10 G60
N11 G0
N12 G93
S500
N13 G98 G84 X-4.5638 Y-3.739 Z-1.3819 R0.125 S500 F.0394
N14 G94
N15 G80
N16 Z0.375
N17 G91 G28 Z0. M9
N18 M05
N19 M01
N20 G91 G28 Z0.
N21 G28 Y0. M5
N22 G90
N23 M30
(ESTIMATED TIME CYCLE 0:00:37 HR/MIN/SEC)
%

AMVERGINO · Aug 1, 2019

JCarroll said:
This works on the one I ran.
Same machine and control.

N1 G0 G90 G40 G80 G17
N2 G91 G28 Z0.
N3 T32
N4 M6(M11 X 1 TAP)
N5 M3 S500
N6 G90
N7 G60
N8 G0 G54 X-4.5638 Y-3.739
N9 G43 Z0.375 H32 M8
N10 G60
N11 G0
N12 G93
S500
N13 G98 G84 X-4.5638 Y-3.739 Z-1.3819 R0.125 S500 F.0394
N14 G94
N15 G80
N16 Z0.375
N17 G91 G28 Z0. M9
N18 M05
N19 M01
N20 G91 G28 Z0.
N21 G28 Y0. M5
N22 G90
N23 M30
(ESTIMATED TIME CYCLE 0:00:37 HR/MIN/SEC)
%

Thanks for responding, so the main difference I see is your commanding a G60 on line N10 and on the G84 your S... is before the F...
other than that I don't see any major differences. I've never used a G60 in the yasnac manual it is defined as a "unidirectional approach"
Is this a necessity to run the tap cycle?
Ill give it a try when I fire the machine back up

Mike1974 · Aug 2, 2019

IIRC You need an M29 Sxxx to start the spindle for tapping as Larry said. This was on a matsurra, Yasnac I80 control. Also I think you need a G95, not G93 for feed per rev OR you can try G94, but you need to adjust your feed move then...

edit: I see it is G93. I don't recall that, but ?? I do remember I had to use M29 though, not sure if it applies to your machine...

Mtndew · Aug 2, 2019

change your G94 to a G95.
You're feeding it at .0591 inches per minute and that's why it's so slow.
You want inches per revolution which is G95.

OR
if you want to stay with Inches per minute then you need to figure out the correct feed for the pitch of the tap.
And since you're going 381rpm, then you want F22.5171 as your G94 feedrate.

JCarroll · Aug 2, 2019

Mtndew said:
change your G94 to a G95.
You're feeding it at .0591 inches per minute and that's why it's so slow.
You want inches per revolution which is G95.

OR
if you want to stay with Inches per minute then you need to figure out the correct feed for the pitch of the tap.
And since you're going 381rpm, then you want F22.5171 as your G94 feedrate.

You are correct.
I quickly posted code using an old IP post that was on my computer at home while I was getting it dialed in.
IPR feed rates are the way to go on this control.

I think I'll go back to lurking. The F360 thread was pretty good but I'm to old for this shit anymore.
Sorry.

Mike1974 · Aug 3, 2019

JCarroll said:
You are correct.
I quickly posted code using an old IP post that was on my computer at home while I was getting it dialed in.
IPR feed rates are the way to go on this control.

I think I'll go back to lurking. The F360 thread was pretty good but I'm to old for this shit anymore.
Sorry.

I think the yasnac I ran did want/default to IPR, just for threading though. IPM was fine for everything else...

Delw · Aug 3, 2019

I am guessing he doesnt know code very well.
and he is relying on what the his software put out. in this case he could be using a fadal post/code generator. as fadal will use the thread lead 1.5mm = 0.0591 or 1/TPI x rpm = feed.
or his post/code generator isnt set up for threading correctly.

I didnt know Mitsubishi controls can use thread lead

AMVERGINO · Aug 5, 2019

Delw said:
I am guessing he doesnt know code very well.
and he is relying on what the his software put out. in this case he could be using a fadal post/code generator. as fadal will use the thread lead 1.5mm = 0.0591 or 1/TPI x rpm = feed.
or his post/code generator isnt set up for threading correctly.

I didnt know Mitsubishi controls can use thread lead

You're Correct I do not know code all that well, I am still learning. That is why I am asking. My yasnac controller does not have a g95 option the F.. code is only for the pitch and .0591 is the pitch for a M10 x 1.5. Supposedly this pitch will be maintained no matter what speed I command the machine (within reason). I can only command solid tap on g93 and solid tap off g94. Then using g84 give all the parameters. Sorry I didn't respond earlier but I was out of town. I will try some of the above mentioned ideas but using g95 will not work.

Mike1974 · Aug 5, 2019

AMVERGINO said:
You're Correct I do not know code all that well, I am still learning. That is why I am asking. My yasnac controller does not have a g95 option the F.. code is only for the pitch and .0591 is the pitch for a M10 x 1.5. Supposedly this pitch will be maintained no matter what speed I command the machine (within reason). I can only command solid tap on g93 and solid tap off g94. Then using g84 give all the parameters. Sorry I didn't respond earlier but I was out of town. I will try some of the above mentioned ideas but using g95 will not work.

So you are saying G95 is not an option on your machine? I am curious what your code looks like for something like face milling a part, or milling a contour. Is it outputting IPR instead of IPM there too?

AMVERGINO · Aug 5, 2019

Mike1974 said:
So you are saying G95 is not an option on your machine? I am curious what your code looks like for something like face milling a part, or milling a contour. Is it outputting IPR instead of IPM there too?

I used the incorrect term.. The yasnac controller has no g95 command. Also M29 has to do with magazine orientation and position and nothing to do with spindle speed. according to the yasnac manual with solid tapping F.. is only Z axis pitch per revolution mm/rev or in/rev. Also the range of the F has to be within .000001 to 7.874015 in. I have it correct in the code basically F.. on this machine is pitch only. I've tried the code that JCarroll posted above and it does the same thing comes down at speed and then slows to a crawl when its actually tapping. His code commanded speed 3x which I felt was redundant. For some reason our machine slows the g84 canned cycle as soon as its initializing before it enters the part and no matter what speed is commanded it slows to what I'm guessing is about 100rpm.

Mike1974 · Aug 5, 2019

AMVERGINO said:
I used the incorrect term.. The yasnac controller has no g95 command. Also M29 has to do with magazine orientation and position and nothing to do with spindle speed. according to the yasnac manual with solid tapping F.. is only Z axis pitch per revolution mm/rev or in/rev. Also the range of the F has to be within .000001 to 7.874015 in. I have it correct in the code basically F.. on this machine is pitch only. I've tried the code that JCarroll posted above and it does the same thing comes down at speed and then slows to a crawl when its actually tapping. His code commanded speed 3x which I felt was redundant. For some reason our machine slows the g84 canned cycle as soon as its initializing before it enters the part and no matter what speed is commanded it slows to what I'm guessing is about 100rpm.

That is weird. I *know* the Matsurra I ran with a Yasnac I80 used an M29 for rigid tapping. I wish I had a code to post but that was some years ago.

Couple questions-

Have you tried hand editing the code to input a G95, say one line before your tapping cycle? I was using a generic post at the time so I hand edited this every time.

So you are saying "code basically F.. on this machine is pitch only" so everything is posted/uses IPR? Interesting for milling (it is a vmc yes?).... On Fanuc (lathe... only??) for threading you can use E instead of F to get to 5 decimal places...

What is in your 'safety line' G20 or G21?

AMVERGINO · Aug 5, 2019

Mike1974 said:
That is weird. I *know* the Matsurra I ran with a Yasnac I80 used an M29 for rigid tapping. I wish I had a code to post but that was some years ago.

Couple questions-

Have you tried hand editing the code to input a G95, say one line before your tapping cycle? I was using a generic post at the time so I hand edited this every time.

So you are saying "code basically F.. on this machine is pitch only" so everything is posted/uses IPR? Interesting for milling (it is a vmc yes?).... On Fanuc (lathe... only??) for threading you can use E instead of F to get to 5 decimal places...

What is in your 'safety line' G20 or G21?

This is a Kitamura MyCenter3x Vertical Milling Machine. M29 is a chip conveyor command says so in my Kitamura manual sorry for the mixup. However, M54 is a rigid tapping M.. in the Kitamura manual but it doesn't explain anything past that. G95 is not on my machine and isn't recognized. The only 2 G codes for solid tapping are G93 solid tap on, and g94 solid tap off. IPM works in everything except solid tapping. In solid tapping I can only input IPR, it says so in my yasnac manual. G94 and G20 are among the default commands on the "safety line" of the machine.

Mtndew · Aug 6, 2019

I'm really confused here. Granted I haven't ran a Yasnac mill control ever, but have ran Yasnac lathe controls before so I'm sort of familiar with them. I know apples/oranges.

You say that your machine only accepts IPR in tapping yet you're putting in a G94 which is IPM.
G95 typically isn't an option and normally is standard on all controls.
G93 is usually Inverse Time feed.
M29 (for fanuc) is the code that "triggers" the rigid tapping motion.

If your machine can't use the above 3 codes, then they must have alternate codes. For example IPR on your mill might be G295 or whatever.
Do you have the manual that shows the format of your rigid tapping cycle?

For my Fanuc mill this is how my tap cycle looks:

N100T1M06( M10 X 1.5 RH TAP)
/M08
(MAX - Z2.)
(MIN - Z-1.)
G00G90G54X0.Y0.
G43H1Z2.
G95
M29S485
G98G84Z-1.R.5F.05906
G80M09
M05
G91G28Z0.
G91G28Y0.
G00G90X-10.
G90
M30
%

JCarroll · Aug 6, 2019

AMVERGINO said:
This is a Kitamura MyCenter3x Vertical Milling Machine. M29 is a chip conveyor command says so in my Kitamura manual sorry for the mixup. However, M54 is a rigid tapping M.. in the Kitamura manual but it doesn't explain anything past that. G95 is not on my machine and isn't recognized. The only 2 G codes for solid tapping are G93 solid tap on, and g94 solid tap off. IPM works in everything except solid tapping. In solid tapping I can only input IPR, it says so in my yasnac manual. G94 and G20 are among the default commands on the "safety line" of the machine.

You should call Gary Frost's people and get their help.
Machinery Sales are/were the Kitamura reseller in California.

1-626-581-9221

AMVERGINO · Aug 6, 2019

Mtndew said:
I'm really confused here. Granted I haven't ran a Yasnac mill control ever, but have ran Yasnac lathe controls before so I'm sort of familiar with them. I know apples/oranges.

You say that your machine only accepts IPR in tapping yet you're putting in a G94 which is IPM.
G95 typically isn't an option and normally is standard on all controls.
G93 is usually Inverse Time feed.
M29 (for fanuc) is the code that "triggers" the rigid tapping motion.

If your machine can't use the above 3 codes, then they must have alternate codes. For example IPR on your mill might be G295 or whatever.
Do you have the manual that shows the format of your rigid tapping cycle?

For my Fanuc mill this is how my tap cycle looks:

N100T1M06( M10 X 1.5 RH TAP)
/M08
(MAX - Z2.)
(MIN - Z-1.)
G00G90G54X0.Y0.
G43H1Z2.
G95
M29S485
G98G84Z-1.R.5F.05906
G80M09
M05
G91G28Z0.
G91G28Y0.
G00G90X-10.
G90
M30
%

So as I said above G94 turns off solid tap mode. The only two G codes related to solid tapping are G93/G94 I'm attaching below the explanation in the yasnac manual for my controller. IPR is used in solid tap you cannot use IPM.

Problems with Solid/Rigid tapping

Plastic

Titanium

Stainless

Plastic

Plastic

Aluminum

Plastic

Diamond

Diamond

Aluminum

Diamond

Stainless

Plastic

Diamond

Plastic

Diamond

Plastic

Diamond

Aluminum

Plastic

Attachments

Similar threads