5 axis cuts in 4 axis format with a 4 axis post

[Mike Whitten CAD/CAM Contractors]

Hello,

 

I am wondering if anyone has noticed any post limitations when doing 5 axis cuts in 4 axis format with a modern mpfan / mpmaster post on a Vertical or Horizontal mill with X2.

 

I have done some stuff a long time ago in V9 and it worked fine so I believe that it should be fine but I have not ran code on a machine tool yet.

 

Has anyone done this type of work with the new Advanced Multiaxis?

 

Thanks in advance!

 

Mike

[Jack Neelands™]

I have not had any problems myself with the Mpfan...I even modified one to suit the horizontal on the floor at Rhocan and tweaked it for non editing....you get to look at it before you send it and that is all you need to do

[cadcam]

There is an issue with the Horz config on how the Machine def is setup.

 

I just was going thru this this week with a customer of mine.

 

I need to put the break down togeather, then I can share.

[Mike Whitten CAD/CAM Contractors]

Jack,

 

Thanks for the tip!

 

 

Jay,

 

I am also having a few issues with the Horizontal. I am busy this weekend helping a fellow machinist move. I will finish troubleshooting it next week sometime and maybe post on this thread.

 

Thanks!

[Jack Neelands™]

Please let us know what toolpaths you are having problems with...ftp site is good to put some close examples without compromising your employer's parts if you wish

[cadcam]

I will post a sample later today after I get back from being out with the family for a while.

[Alvaro Gil - Cimquest-inc.com]

Im having the same issues. Cant get B axis output (rotary axis on the Y) when using a 5 axis toolpath. X works ok but when you change the machine def to rotate about the Y axis, and you create a 5 axis toolpath locked to the Y axis (the only option) it does not output any B codes.

 

Let me know if you figure this out.

[gcode]

You have to set up a false axis in the machine

definiton to make 5X cuts work on a 4axis machine.

Otherwise, the toolpaths backplot correctly

but all the posted output is relative to the top plane.

I've got the files and details at home.

I'll see if and can find them and post more this evening.

[Mike Whitten CAD/CAM Contractors]

Alvaro,

 

The problem I was having was when doing a Five axis cut in four axis format with an X2 post it would not work. If I used an updated 9 post with the CD/MD set up the same it would.

 

What we got from CNC's post department was that it was a bug in the post which just a one line change. I tried it and it worked. The fix was supposed to be in MR1 (mpfan). Run a compare and see. Let me know if you need it. I am on a hot job so I must go

 

Mike

[88Matt]

Same here. We are currently using a v9 updated post on our 4x horiz Mori. At first we had the same prob. rotation was locked on A. Changed the machine def then worked fine. Can you share the fix? I would like to switch to the newer defs and posts.

 

Thanks

[Mike Whitten CAD/CAM Contractors]

Here are the fixes for Generic Fanuc 4X Mill.pst The fixes are supposed to be in MR1. The additions are in bold.

 

# CNC 10/06/05 - Changed parameter read for min_speed, modified pspindle, pprep$ and pset_mach

# - Modified pset_rot_label to use srot_y for horizontal machines

# - Added call to pset_mach in pq$ to set rotaxtyp$

# CNC 11/18/05 - Added psynclath with call to pset_mach to set rotaxtyp$, removed call from pq$

# CNC 02/03/06 - Added logic for high-speed toolpath tool inspection (see prapidout & plinout)

# CNC 06/26/06 - Initial post setup for Mastercam X2

# CNC 12/15/06 - Modified pset_mach for horizontal rotation when rotating about world Z axis.

#

# --------------------------------------------------------------------------

# Features:

# --------------------------------------------------------------------------

# This post supports Generic Fanuc code for 3 and 4 axis milling.

# It is designed to support the features of Mastercam X Mill.

 

rd_mch_ent_no$ = syncaxis$ #Retrieve machine parameters based on current axis combination - read from .nci G950 line

rd_md$ #Read machine definition parameters - calls pmachineinfo$

 

#We only need these set at toolchange (and start of file). No need to set them each time a user may call rd_md

rot_on_x = rot_axis

if not(vmc) & rot_on_x = 3, rot_on_x = 2 #If HMC and rotating about world Z axis (machine Y axis)

rot_ccw_pos = rot_dir

index = rot_index

if rot_angle = zero, ctable = one #ctable zero will produce a divide by zero error, so force to one if zero in MD

else, ctable = rot_angle

 

if met_tool$ = 1,

 

 

Mike

[Guest CNC Apps Guy 1]

You HAVE to do things new school, eg. Front = B0, Right Side = B90, Back = B180, Left Side = B270, etc...

 

If you don't use this setup, you'll have issues.

[Mike Whitten CAD/CAM Contractors]

James,

 

What are you saying? Please give me a hint.

 

Mike

[crazy^millman]

Well you would have to know that James for years did his like a VTC set-up in Mastercam and before MD it did not matter since they have Machine Definitions you can not get away with that so when doing 4th have HMC work correctly from Mastercam you have to d oit like looking at the machine. Like using front for A0, Right for B90 like he was saying. James and others I have known did it as Top was A0 on the HMC and Front was B90 and so forth. This worked and when changing from a VTC to HMC with the same file you never had problems. Now if doing 4th axis work between machines you either need to do it 2 ways or use a WCS for one set of operation and then copy the operation and use another.

 

What I have been doing for a files that are posting for different machines is make the file for the machine then add several machine defs and the copy the operation to each one update as need to and go from there.

 

HTH

[Mike Whitten CAD/CAM Contractors]

Ron,

 

I am aware of the way James liked to do it but never thought about how he was doing it now with the new stuff.

 

I thought he may have been talking about the fact that the WCS will not work correctly with multiaxis cuts. This is a bummer also.

 

Thanks,

 

Mike

[crazy^millman]

Could be as well and really maybe speaking out of turn since James is really the only that know what he is thinking not anyone else.

[gcode]

quote:

---

I thought he may have been talking about the fact that the WCS will not work correctly with multiaxis cuts

---

I've had good luck with WCS and 5X postitional

cuts.

[Mike Whitten CAD/CAM Contractors]

gcode,

 

I will have to look at that again. I tried some simultaneous milling with the Advanced Multiaxis quite some time ago and I could not get it to work so I had to move the part. Maybe I did something wrong. I will check it out again.

 

Thanks,

 

Mike

[cadcam]

So james you program the 4th in the old style (This comment is not a slam james it's just what I call it)of Virtical and not as a Horz. so top is what you program instead of Front like a Horz. Am I catching you correctly?

[Guest CNC Apps Guy 1]

quote:

---

...So james you program the 4th in the old style...

---

I did... up until WESTEC. When I tried to do some Simultaneous 4 Axis stuff(with a 5 axis toolpath) for a demo... found out I had to change my old ways (which BTW I'm not happy about because there's NOT A SINGLE GOOD reason why I should not be able to do it the old way which is BY FAR more flexible). But it is what it is. I'm not taking it as a slam against me. You new school guys should be telling me get with the program ya friggin old timer!!!

 

I like Top as B0, Create a plane for B90, Bottom as B180, and Create a plane for B270. That way it is in the system as it is in the machine, AND i can easily transport programs between VMC's and HMC's.

 

The new school method is for folks too lazy to create their own planes IMNSHO!

[Greg Williams]

quote:

---

I like Top as B0, Create a plane for B90, Bottom as B180, and Create a plane for B270. That way it is in the system as it is in the machine, AND i can easily transport programs between VMC's and HMC's.

---

This is how like to do it!

 

Seems like we take 1 step forward 3 back, Dear oh Dear does the ship have direction?

[gcode]

Mike,

sorry I'm so tardy getting back to you.

I sent a detailed description of the workaround

to the email address listed on your profile.

Hope it helps

[Mike Whitten CAD/CAM Contractors]

gcode,

 

I did get the email. Thanks!

 

I was able to get around the issue with the info we got from CNC as I listed above. I will have to study all of this when I get a little time. I will let you know.

 

Thanks,

 

Mike