Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Fanuc G68.2 with rigid tapping


g huns
 Share

Recommended Posts

After much d!cking around with Fanuc, Enshu, and our non-Mastercam software provider, I thought I had G68.2 and TCP control all figured out for our two horizontal machines. COR is good, post is working fine, test cuts all worked great.

Then we tried to cut a real part.:rolleyes:

The machine errors out when we attempt to rigid tap while the tilted work plane is active...

M906T154
S145 M3
T46
G0 B90. 
G68.2 X7.38189 Y0. Z-1.57116 I90. J90. K-90.
G53.1
X0. Y.02165 
G43 Z3. H154
M8
(AUTO_DRL)
G94
M29 S145
( MOVES TO X Y POSITION  Z.200 AND ALARMS )
G84 G98 X0. Y.02165 Z-.7 R.2F10.0000
G80
M19
M9
G69
G05.1 Q0
G91 G30 Z0.
G90
M01

Here are the alarms...

 3bwELGY.jpg

All other drilling cycles seem to be working. Does the 'Y' in the first alarm indicate the Y axis? Why would a rigid tap cycle trigger a Y axis alarm?

Of course Fanuc is utterly useless for help. Enshu has never had TWP installed on a machine so they know nothing. And our post writer says this post works for his customers running OKK and Makino horizontals.

Link to comment
Share on other sites
1 hour ago, Colin Gilchrist said:

Are you cutting a Metric thread? I'm trying to figure out what Tap has 14.5 TPI?

A Metric Pitch of 1.75mm would get you there, I'm just curious...

10 / 145 = .0689655172413 Pitch.

.0689655172413 x 14.5 = 1.00000000000001

Yep. M12x1.75.

  • Thanks 1
Link to comment
Share on other sites
6 minutes ago, g huns said:

There's a G17 at the beginning of the program. I guess another one can't hurt.

we've got a couple of Fanuc 31i's that support G68.2.

I've found that it's usually best to force a G17 every time you define and  move to a G68.2 work plane 

Most of the time, it make no difference at all, but sometimes it makes a difference

Link to comment
Share on other sites
2 minutes ago, Colin Gilchrist said:

Dude,

I think it is the G68.2 rotation. I don't believe I've ever seen these used like this:

I90. J90. K-90.

Typically, one of these is "0.", but it really depends on the order that the rotations are applied to coordinate system.

This is a 4 axis horizontal machine, if that makes it make any more sense. I honestly don't even try to wrap my head around what it's doing.:blink:

All I know is the tap drill cycle worked fine right before this. Only rigid tapping is a problem. Like maybe it thinks it's tapping in Y instead of Z? But the G53.1 should make that all good.

Link to comment
Share on other sites
3 minutes ago, Colin Gilchrist said:

Also, not sure this is causing the Tapping error, but you'll need a G49, before the G69.

Haven't needed it yet. And we have run on multiple sides of a block using multiple G68.2s.

  • Like 1
Link to comment
Share on other sites

For your G68.2, we are using the "P0" method. (P0 is assumed, when omitted, so we are using Euler Angles for rotation.)

Check if this makes sense on your machine for how the coordinate system is aligned. Your machine may be going to the correct "position", but it may think the Coordinate System Axes are not aligned so that the rotated "G68.2 CSYS Z Axis", is aligned with the spindle.

For Euler rotations, here is what the IJK Values represent:

I = Z Axis Rotation, about the MCS "Z" Axis. This is "Rotation 1". After Rotation 1, we have CSYS X'Y'Z'. (read as X prime, Y Prime, Z Prime) These are the rotated XYZ unit vectors.

J = X Axis Rotation, about the X Axis, of X'Y'Z' CSYS. This is "Rotation 2". After Rotation 2, we have MCS X''Y''Z''. (X double prime, Y double prime, Z double prime).

K = Z Axis Rotation, about the Z Axis of the X''Y''Z'' CSYS. This is "Rotation 3". The final rotation is used to rotate the X''Y''Z'' CSYS, so that the X Axis Vector Direction of the X'''Y'''Z''' (triple prime) CSYS, is aligned to the X Axis of the Machine. This last step is crucial, so that the CSYS created is "oriented" to the machine CSYS in a way that makes sense.

 

Link to comment
Share on other sites
7 minutes ago, g huns said:

This is a 4 axis horizontal machine, if that makes it make any more sense. I honestly don't even try to wrap my head around what it's doing.:blink:

All I know is the tap drill cycle worked fine right before this. Only rigid tapping is a problem. Like maybe it thinks it's tapping in Y instead of Z? But the G53.1 should make that all good.

I took a look at the ZXZ rotations, and those rotations are actually correct.

Link to comment
Share on other sites
8 minutes ago, Colin Gilchrist said:

(P0 is assumed, when omitted, so we are using Euler Angles for rotation.)

I would agree that the angles are odd being 90,90,-90  but those make sense for working on the side, with Euler Angles.  What I am having trouble picturing is B90 the left side or the right side.  Looking down on the tombstone, does it turn clockwise or counter-clockwise.  It's been too long since I have been on a horizontal.

Link to comment
Share on other sites
1 minute ago, huskermcdoogle said:

I would agree that the angles are odd being 90,90,-90  but those make sense for working on the side, with Euler Angles.  What I am having trouble picturing is B90 the left side or the right side.  Looking down on the tombstone, does it turn clockwise or counter-clockwise.  It's been too long since I have been on a horizontal.

The problem is...

 

the direction is controlled by a Parameter. So what is +90 on your machine, might be -90 on mine...

Link to comment
Share on other sites
9 minutes ago, huskermcdoogle said:

Just for kicks, try a regular old G84 without rigid.

Another thing to think about, do you have bit 1(LRP) of parameter 1401 set to 1 or 0?

It's a 1.

2 minutes ago, Colin Gilchrist said:

I took a look at the ZXZ rotations, and those rotations are actually correct.

I'm glad someone understands it. I feel like a total dumbarse every time I try to make any sense out of it.:wacko:

 

2 minutes ago, Colin Gilchrist said:

Is your High Speed Machining code active? I see a G05.1 Q0. after the G69...

No. Our post just outputs that G05.1 Q0 at the end of every program.

 

Just now, huskermcdoogle said:

Totally concur.  This has go to be a stupid parameter issue.

On another note, has any rigid tapping been done without G68.2 active?

I agree. And since Fanuc couldn't even get the major ones right to make TWP and TCP work, I doubt they are gonna fix this either.

Yes. Rigid tapping is no problem when NOT using TWP.

Link to comment
Share on other sites

I'm reasonable certain the G68.2 code is being output correctly. I say that because:

  • The machine moved to the correct "starting position" in XY prior to the Canned Cycle Call.
  • The machine moves into position at Z3.0 to before the cycle starts.
  • He has a "R.2" in the code, and the machine rapids down to "Z.2", then errors out.

Those things together tell me that the machine coordinate rotation was correct.

Link to comment
Share on other sites
14 minutes ago, Colin Gilchrist said:

I'd keep escalating this with the MTB, until they fly out someone who can make it work.

Me, the guy from Cimatron who wrote the post, his customer with a Makino running his post, the world famous James Meyette, and some eMC help is the only reason TWP and TCP work at phuking all. 

Literally, the only parameters the Fanuc guy set right were the ones that enabled TWP and TCP as options.

I cut our MTB a lot of slack in this. They have never had these options installed on one of their machines. I don't even think they understand what they do. After dealing with Fanuc, I think you can count on one hand the number of people they employ who understand it all. And they don't send those guys out on service calls.

I think most of knowledge about this stuff resides with MTBs that install these options frequently.

The president of Enshu is coming over from Japan to visit later this month. He will be hearing a lot about it.:angry:

  • Like 3
Link to comment
Share on other sites
41 minutes ago, g huns said:

I think you can count on one hand the number of people they employ who understand it all.

It's also quite possible they don't have any one person in the country that does.

Everyday I think it would be infinitely valuable to become one of the guys who understands the Fanuc control options inside and out.  I would think that if you could get Fanuc to "hire" this person on commision sales only, they would be free to run around the country consulting on options to reduce cycle time or solving customer application issues like this for hourly fees, Fanuc would get a small cut of the hourly fees, if no option sale is being made.  Fanuc would back them with any documentation they need and give them the ability to go direct to Japan for assistance when needed. This person would also be able activate and install options for testing purposes.  Of course Fanuc would be tied into this, but no extra service call would be needed to do it, and the customer could see right then and there with confidence if the option is really worth the money or not.  MTB's especially ones that are made overseas, but have a US based sales and support organizations would love to have someone like this available for those special off the wall projects that need to squeak just a little more cycle time out of the machine.

If these people existed, I think many shop owners pocket books would open up and start "optioning" out their controls.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...