×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Best way to program 4-axis horizontal mill NX6

Best way to program 4-axis horizontal mill NX6

Best way to program 4-axis horizontal mill NX6

(OP)
HI,
I was looking for the best way to program toolpaths for a 4-axis horizontal mill with a B-axis rotary table in NX6. What I am trying to do is fairly basic: mill the first face with planar operations then rotate the table CCLW 90 degrees and proceed to milling the second face with planar operations as well. I was able to insert a ROTATE event after the first set of operations, but when rotating it produced a crashed "workpiece against toolholder" on my machine simulator. So I was hoping I could get some input from those who have done similar programs.
thank you.

RE: Best way to program 4-axis horizontal mill NX6

The tool axis position should cause B axis rotation.  You should not need to put in a ROTATE command manualy.
For the second operation set the tool axis normal to the floor face.

If you post is correct you should get a B axis move

 

John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO
www.myigetit.com

RE: Best way to program 4-axis horizontal mill NX6

(OP)
John,

I tried what you suggested and it does rotate without having to insert the event manually. So thank you for that. However, I still have a collision between the tool and the IPW. Any ideas how to avoid collisions?
Thank you

RE: Best way to program 4-axis horizontal mill NX6

When are you having a collision?  When you rotate?

Make sure you retract the tool far enough away between operations.  You can set the Non-cutting moves for the final departure to move the tool to a clear location.  You can also add a Machine Control opertion with a goto move to position the tool.

 

John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO
www.myigetit.com

RE: Best way to program 4-axis horizontal mill NX6

I concur with what Joycejo implies by setting a clearance plane, which is under the Avoidance menu options.

Alternatively, you could reconfigure your post-processor, as my last company did on a Matsuura MC900-HG horizontal machine to retract all of the machine axes to machine-home positions (or some other safe position before any rotational B-axis moves - much safer.

RE: Best way to program 4-axis horizontal mill NX6

(OP)
John,

yes, the collision occurred when it rotated 90 degrees. Would you mind clarifying what you mean by adding a GOTO move as a machine control operation?


XFV8,

Would you be kind enough to tell me how to do that in Postbuilder?

Thanks

RE: Best way to program 4-axis horizontal mill NX6

Would you be kind enough to tell me how to do that in Postbuilder?

I wish I could, but I've never been trained on Post Builder.sad

Essentially, the sequence is as follows:-

1. Retract the tool axis (Z) coded G91 G0 G28 Z0

2. Move X an Y axes to safe position, (in my case G91 G0 G28 X0 Y0)

3. Unclamp the B-axis, (M22)

4. Specify the new B-axis position and new fixture offset
   if you're using multiple machine offsets, i.e (G54.1 P2 B0.)

5. Clamp the B-axis (M23)

6. Respecify your tool length offset, (G43 H05 Zn.nn)

...and so on. Maybe someone more experienced in PB will be along soon.

RE: Best way to program 4-axis horizontal mill NX6

I would steer clear of adding "Machine control" events. There are more elegant ways to stay safe.

I included a .jpeg showing 2 easy ways to stay safe.

1. Set your automatic retract to a safe distance in the WCS dialog. Just make sure that all your operations use that particular WCS and they will all inherit the clearance.

2. Add a "go home" block to the end of operation event in postbuilber. The tool will go home after every single operation(with or without an axis change). Very safe. a good opportunity for machinists to check inserts/tool wear aswell.

Now, these are only 2 suggestions. There are many, many, many more ways to get what you want.

Disclaimer: If you edit your post, be very, very carful. Double check your code! then check it once more... ;)

J

RE: Best way to program 4-axis horizontal mill NX6

(OP)
Thank you gentlemen, I will give it a go!

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources