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:

New Fanuc Robodrill G53.1?


Recommended Posts

Hi Guys

Anyone in here with programming experience on Fanuc Robodrill with 4th axis? It's an 31i B5 control.

I'm new to programming on Fanuc and i'm trying to get the MasterCam Post Processor working.

I've made a simple program with tilted "B" axis in 57degrees. (I know i should be "A" but apperently thats the way Fanuc makes it!)

If I delete G53.1 it works, but isn't it necessary?

Also if you see any other problems in my program please let me know ^_^

 

Regards

Jacob

 

 

test.txt

Link to comment
Share on other sites

Sounds like the option for G53.1 was not purchased and you got an alarm when you tired to run it? Ask the builder to supply you with a proven program for that machine and then use it to to come up with the output you need. G53,1 is more for 5 Axis machine and may not needed on a 4th, but is used more with G68.2 like in your example. Again every machine is different and where the builder should be able to help you sort this out with a phone call. Normally G53.1 is on a line by itself without the P1 output.

You say it should be A axis and the 4th Axis is along X and not Y axis correct? I thought I was X for J was for Y and K was for Z for Axis rotations. Yes I see J57. which tells me the MMD is setup for rotation along the Y axis not the X which confuses me since you said it should be A axis which would be along the X Axis for rotation and I would expect to see I57. not J57.

Link to comment
Share on other sites
3 hours ago, C^Millman said:

Sounds like the option for G53.1 was not purchased and you got an alarm when you tired to run it? Ask the builder to supply you with a proven program for that machine and then use it to to come up with the output you need. G53,1 is more for 5 Axis machine and may not needed on a 4th, but is used more with G68.2 like in your example. Again every machine is different and where the builder should be able to help you sort this out with a phone call. Normally G53.1 is on a line by itself without the P1 output.

You say it should be A axis and the 4th Axis is along X and not Y axis correct? I thought I was X for J was for Y and K was for Z for Axis rotations. Yes I see J57. which tells me the MMD is setup for rotation along the Y axis not the X which confuses me since you said it should be A axis which would be along the X Axis for rotation and I would expect to see I57. not J57.

Thank you very much.

Yes the 4th axis i along X and it makes perfectly sense that it should be I57 instead. We have had some issues with the builder because they're very very slow  to reply when contacted. Fanuc will send a technician tuesday because they suspect that the parameters on the machine is not set up properly.

Link to comment
Share on other sites

When using G68.2, it is necessary to use G53.1 on a Table/Table type machine. THis is what tells the control the spindle's orientation. The function is called Tool Posture Control. 

Link to comment
Share on other sites
On 5/24/2017 at 10:57 PM, Foghorn Leghorn said:

The function is called Tool Posture Control. 

Well technically it is called Tool Axis Direction Control.  G53.1 moves the machine such that the tool axis is perpendicular to the machining feature plane that was described and set using G68.2.   As you probably know Tool Posture Control is an entirely different function which, and correct me if I flub this up, is a subset funcion of G43.4/G43.5 commanded using a P1 on that command, which controls axis posture between programmed points to maintain intended planar or conical geometry without a having to calculate intermediate points and angles.  The intention of it is make it easier to program in five axis without CAM and/or to allow for smoother motion more accurate to form machining between defined points in the CAM program.

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...