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:

NTX2000 G68.1 issues


Bob W.
 Share

Recommended Posts

We are doing some milling at 45 degrees using the upper turret on our Mori NTX2000 and things aren't behaving as expected.  The tool position is off in X and Z by 1/2" or so. Here is the cod3

T6603
G361 B-45. D0
G43 H1.
G97 S4075 M13
G54
G98
M69
G0 C180.
M68
G17
G68.1 X0. Y0. Z0. I0. J1. K0. R45.
M08
G0 X-2.3559 Y-1.0523 Z5.
Z2.9086
G98 G1 Z2.8106 F100.
X-2.3536 Y-1.0513 F75.
X-2.3048 Y-1.0221 Z2.8101

From what I can see everything looks right.  The rotation is at the G54 XYZ 0,0,0 position and rotating 45 degrees about the y-axis.  When I take measurements in Mastercam the tool position matches where it should be relative to the G54 origin but on the machine it is a different story.  Are there Fanuc parameters that need to be set for this?  It is a 2D HST contour toolpath so no wear comp, etc...  Also, the machine didn't like I,J arc moves and alarmed every time but linear code ran well.  Are arcs in G68.1 an issue?

Link to comment
Share on other sites

Wait I just noticed G68.1 and not G68.2. Do you have a copy of the programming manual for that machine? I always equated G68.1 with rotation on a normal plane not 3+2. Is it G68.1 or G68.2 and you mistyped? If not then try changing that to G68.2 and using the arcs and see if the machine alarms out then. 

G68.2 or TWP (Titled Work Planes) is that anything you would normally do in 3 Axis can be easily programmed the same way and the rotated to the new 3+2 positions and done. Originally it was developed for programming by hand at the machine in a titled plane without having to Trig everything out. The other advantage is most canned cycles are not written to support more than Single plane process. A Canned cycle for the most part is a single plane process. It follows the Vector and that it is. The exception being the boring cycles that will shift the tool, but it still stays in the same original vector. just like the 3 Axis programming being able to change planes with G68.2 the canned cycles also benefit from that. Again when we were doing this by hand we either moved the part to use 3 Axis process or we Trigged it all out to do this. With G43.4 you are getting long code for the drilling cycles which is not a big deal, but tapping is where it becomes an issue. Everything else can be a canned cycle or long code. The issue I have with a lot of Fanuc builders is their poor implementation of G68.2. On a Heidenhain or Siemens control they handle TWP very nicely. On the majority of Fanuc control you have to share the same WCS for the G68.2 and the G43.4. With that then the code much match. With the other controls you have a lot more control and power to have one WCS values and as many Tool Plane values as you want. The Datum C is 20" in X, 40" in Y and 2000" in Z from the WCS then the G68.2 line is X20. Y40. Z2000. I0 J0 K0 R45. then all your programmed values on 1" deep from that Datum C like on your print and just that Z-1.0 for a depth. Not 2000" plus some rotation from the original Zero. Now I get it who cares code it code, but when you have people always 2nd, 3rd, and 20th guessing what you do having better options for posted code it not a bad thing. 

TCP is G43.4 which is Tool Center Point Control or Cutting Point Control and with that you can do whatever you want, but expect program to be much larger. 

Link to comment
Share on other sites

Yes, it is G68.1 which seems to be a less powerful version of G68.2 though better than G68.  G68.1 has the same inputs as G68.2 and the Mori AEs say it is typically used on these.  With that said this machine has all of the 5-axis options so we could run TCP, TWP, etc...  but I'm not sure the post is set up for it and there is a lot more complexity there that I don't want to deal with at the moment. 

Link to comment
Share on other sites
On 10/23/2020 at 2:49 PM, Bob W. said:

Yes, it is G68.1 which seems to be a less powerful version of G68.2 though better than G68.  G68.1 has the same inputs as G68.2 and the Mori AEs say it is typically used on these.  With that said this machine has all of the 5-axis options so we could run TCP, TWP, etc...  but I'm not sure the post is set up for it and there is a lot more complexity there that I don't want to deal with at the moment. 

Bob, yes the post is setup to support full 5 axis work and should do so with no issues on that machine.

Have the Mori AE give you proven code and go try to run it on the machine. Compare it and see what the difference are. That is normally what I have to do every time a customer runs into issues with a machine.

Link to comment
Share on other sites

I use G68.1 a lot on the NTX2000, and this is an example of simple milling operation on the sub spindle. Make sure that you set the tool offset correctly. The I, K work fine on my machine.

T---

G361B30.D0

G43H----.

G97S3056M13

G55

G98

M269

G0C66.5

M268

M484

G0G17Z1.3078

X5.5515Y0.

G68.1X0.Y0.Z0.I0.J1.K0.R120.

G0X-5.0409Y0.Z1.75

Z.3629

G18G2X-4.455Z.4987I-.7979K2.1038F30.

G98G1X-1.5163Z1.3132

G0Z1.75

X-5.1513

G17Z.3064

G18G2X-4.42Z.4684I-.7252K2.1299

G1X-1.4813Z1.2829

G0Z1.75

M269

G0C21.5

M268

  • Like 1
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...