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:

Rotary 4th Axis Posting


toolbreaker
 Share

Recommended Posts

Using Rotary 4th axis programming with V8 for the first time and having problems with the posting (I think).

Using the mpmaster post downloaded from this site but despite graphically everything seeming okay in the nci file in MC backplot (animated) and MC verification as well as Predator VCNC (to double check) all goes wrong on the m/c. The rotary axis is configured to rotate the correct direction (as programmed) but axis positions are clearly not correct. Sort of right but completely wrong if you know what I mean!! - but not a tip/centre compensation issue. The result is the same with the mpfan post.

I imagine there must be something really basic I am missing - maybe something to switch in the post.

Never had a posting problem previously - any tips??

Help............

------------------

 

Link to comment
Share on other sites

I've done limited 4X work, but the post worked. When you are drawing your geometry,

you have to set your Z level to the radius

of your work

If you are working on a 4in dia part draw

your geometry a Z=2.00

When your are touching off the cutting tools be sure to add the radius of the part to your Z offsets. The post outputs with the

C/L of the 4th axis as Z zero.

Link to comment
Share on other sites

toolbreaker,

The mpmaster post is 4X enabled.

Look at the third line of the

"Rotary Axis Settings" in the post

If you are not getting an A command

in the first rapid move of any tool path

(even a regular 3X program), the 4X switch has been turned off.

 

 

Link to comment
Share on other sites
Guest CNC Apps Guy 1

For BEST results, draw everything as it will sit in the machine AND make sure the centerline of rotation is correct. If this is not right, you'll surely have problems.

The way I have done 4 Axis Programming in the Past (And been quite successful I might add) is to model the tombstone, and any work holding devices that may be part of the setup. Draw the part sitting as it would in the fixture. Yes I know it is time consuming but the results will be what you are expecting and will be much more predictible.

James Meyette

[This message has been edited by James Meyette (edited 02-03-2001).]

Link to comment
Share on other sites

Okay,

Just to clarify...no problem creating lovely grahic rotating images, looking good in both MC backlot and verification - great, but the problem arises for me during the messy business of actually cutting metal.

Maybe the question should have been: Has anyone actually had experience of using the mpmaster post for generating good quality simultaneaous 4axis code? (not just as an indexing instrument)

I've never previously had any problems whatsoever with MC posts with the code always xxxx on, but this is my first attempt at simultaneous 4axis and have built up a confidence (mis-placed?) that if graphically everything was right that the code could be expected to be correct. So, I was somewhat stuck for ideas (to say the least) - confidence shattered! - when the finished article was not a patch on my graphically perfect demonstration.........Could it be just a post limitation (or its not very good for complex work) or have I just plain forgot to do something necessary within the post configuration I wonder?

------------------

 

Link to comment
Share on other sites
Guest CNC Apps Guy 1

Okay, I think I get it.

You're using MPMASTER post? I am not familiar with that post. Mastercam does very well at FULL rotary motion. The problem most likely resides in your post.

From your main menu, go to Flie, Edit, Pst, and then pick out the post you are trying to use, at the top of the post, it shouldtell you what is supported for example see below,

# Customer : XYZABC Engineering

# Post Name : MPFAN16i

# Product : MILL

# Machine Name : Mori Seiki SH-630

# Control Name : FANUC 16iMA and 18iMA

# Description : Horizontal Mill Post

# Associated Post : MPFAN

# Mill/Turn : NO

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Executable : MP 8.00

As you can tell, this post supports 4 axis and 4 axis sub programs as well as standard sub programs but does NOT support 5 axis.

I have used the MPFAN right out of the box and created Full Rotary motion programs that have worked (with of course the tool changes modified for the specific machine)

Your post should have the general information about what it supports in this section. If you read further down (in your actual post, you'll find out how to use the Misc. Reals/Integers to acheive specific things, like G28 or G30, or G92 or G54 etc...

Let us know what you find there.

James Meyette

[This message has been edited by James Meyette (edited 02-04-2001).]

Link to comment
Share on other sites

toolbreaker;

Sorry, my problem is with MC v7.2c. It may have been corrected in v8.

I was only suggesting that it may be a 5-axis post problem because the NCI g-code for a Rotary 4-Axis toolpath is G11, which, as my post processor user guide inticates, is a 5-axis move which may require a "special" post processor. Don't ask me why, that's what it says!!! There doesn't appear to be a seperate g-code for a 4-axis toolpath.

 

 

Link to comment
Share on other sites

JM,

Its good to hear that you have achieved some good code using mpfan.

mpmaster is just an enhanced mpfan, and my initial problems was the same with both posts.

I've gone back to basics and taken a path off a straight forward cylindrical model (50mm dia x 50mm L, 6mm BN x 2mm stepover) just to make the code reading easy.

Haven't cut metal but the code would seem to be okay with a correct z axis movement to the od and the a axis incrementing at 4 1/2 (approx) degree increments per line. The angle of rotation continues totalling up (not limited to 360 deg) until the end of the path.

I assume that despite the angular line incrementation tool movement would flow.

The only other query was the first axis movement which was to -47deg as a start pos'n which seemed a bit odd but I assume is as a function of a length/step over calculation?? - I'm guessing - not really an issue if the end result is okay.

Hopefully I can get it on a machine shortly.....

Thanks to all brainstormers, the input is appreciated...

------------------

 

Link to comment
Share on other sites

Indeed Mpmaster is a 'child' of Mpfan, with some minor changes, additions, rearranging, etc. Handling of rotary moves should be identical.

V8 posts related to Mpfan will support rotary substitution, rotary indexing, and the NCI gcode 11 5-Axis style move (without any support for side to side tilting of the tool vector). Peter is correct in that some V7 posts may not support the NCI gcode 11 5-Axis style move. They can of course be modified to do so.

Keep in mind that not all machines use unlimited absolute positioning rotary axis. A machine may use a direction sign coupled with an absolute 0 to 360deg position as an example. +/- directions may also need to be changed in the post.

The first move in a rotary program will typically take the shortest move to correctly position. -47deg is a shorter move than +313deg.

Link to comment
Share on other sites

For the VMC configuration (vmc : 1), and the rotary axis rotating about X (rot_on_x : 1), the tool in the Top toolplane is considered to be at A0. The tool in the Front toolplane is considered to be A-90 for a CW positive A-Axis (rot_ccw_pos : 0). or A90 for CCW positive A-Axis (rot_ccw_pos : 1). Without these absolute position defined with respect to the Top toolplane reference position, it would be impossible to use a rotary operation in the context of larger file with other operations.

Link to comment
Share on other sites

DT,

Appreciate what your saying which is fine.

But, in the basic test piece we are dealing with, a 50mm perfectly round (in section)cylinder, VMC, X axis rotation setup, Top Tool plane machining only, would you expect to see an initial axial movement of -47 deg? I did not and expected an A0 start position.

This may or may not be related to the overall problems, I don't know, and I would not be overly concerned where MC decides to start the cycle as it should be m/cing thro' 360deg anyway (if the finished component is correct).

------------------

 

Link to comment
Share on other sites

I'm not positive of what you are talking about....but I know when I program rotary moves, if I don't start machining at rotary 0, Mastercam automatically makes my first rotary move 0. So to eliminate the problem I always run a tool at rotary 0 (a drill), and put a note with it that says DELETE, and after posting, I delete it. It's the only way I know of telling mastercam where rotary "0" is.

Frank

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...