5 Axis - Resolved to 4 axis

[Mick]

Hi there,

 

We have a surface machining operation, which is a sloping surface, which we are machining on a Toyoda FA1050S horizontal machining centre.

 

The part is programmed using 5 Axis flowline. The toolpath looks fine, but when it is backplotted, the part flips to the "back". When the posted code is run through vericut, it appears to be machining the part mirrored about the machines Y axis.

 

We are using a toolplane defined off the sloping face (the sloping face is 25 degrees off B0)

 

The tool axis curves are defined correctly. What could we be doing wrong? Does anyone have any suggestions?

[Bruce Caulley]

Have a file you could share?

[Ron Branch @ Verisurf]

Never Trust Mastercam to be right always trust Vericut. Turn the Plane 180 degree repost and see what it looks like in Vericut. Vericut is going ot be right where Mastercam screen shot can be wrong and trick you into crashing the machine.

 

HTH

[Mick]

I do have a file I can share. If anyone wants a look, post up your email address

 

Ron, yes, I might try that

[Mike Whitten CAD/CAM Contractors]

Hello Mick,

 

I have done several parts in X2MR2 that had quite a bit of 5ax cuts in 4ax format on HMC's. I have always set the TP to Front and used a standard mpmaster post.

 

There was an issue in the mpfan based posts..maybe it was early X2 that would cause a serious issue. You can search for this if you want.

 

I would suggest to just take a late model mpmaster post, set my TP to front and try it again.

 

Thanks,

Mike

[Mike Whitten CAD/CAM Contractors]

Mick,

 

I just researched the post issue just in case that's the issue causing your problem. The "Generic Fanuc 4X Mill.pst" was missing an important line of code in the first X2 release. I believe it was fixed in X2 MR1. My guess is that mpmaster also needed the same line of code. The following below was copied from an old post I put up back then.

 

The fix came from CNC for the "Generic Fanuc 4X Mill.pst" 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

[Mick]

What is weird, is that when I backplot the part, it flips the part around, even though the part is sitting in the correct orientation. This is evident when the code is posted, and then run through Vericut.

 

I dont think it is a post issue, but something to do with the planes.

[Mike Whitten CAD/CAM Contractors]

Mick,

 

I will look at the file if you email it to me.

 

edit: I only have X2MR2

 

Thanks

[Mick]

Mike, I'll redo in X2 right now, and email it to you. I appreciate you looking at it.

 

It has me beat, as I've tried everything

[Mike Whitten CAD/CAM Contractors]

Hello Mick,

 

I can't sleep tonight so I just checked out your file.

 

Here are a few things I see:

-The backplot seem fine to me.

 

-If I measure a tool vector(saved as geometry)at roughly the smallest and largest B move, it appears to be about the same as the gcode. B51.427 to B75.009

 

-I posted the code two ways. The first way was with the TP origin set as supplied (as you had it) and the other way was with it set to zero. The code looks like it is considering the origin at post processing.

 

gcode with origin as supplied:

G00 G17 G90 G54 B51.427 X-107.646 Y-.004 S3000 M03

G43 H1 Z40.899

Z-54.101

G94 G01 X-102.789 Y-.003 Z-55.286 F300.

X-102.808 Y2.919 Z-55.299 B51.428 F1000.

X-102.859 Y5.882 Z-55.332 B51.431

 

gcode with origin set to zero:

G00 G17 G90 G54 B51.427 X161.214 Y-.004 S3000 M03

G43 H1 Z824.055

Z729.055

G94 G01 X166.072 Y-.003 Z727.87 F300.

X166.039 Y2.919 Z727.862 B51.428 F1000.

X165.946 Y5.882 Z727.843 B51.431

X165.806 Y8.884 Z727.818 B51.436

 

X161.214 is about where it should be according to what I see.

 

The WCS origin and TP origin should be set to the center of rotation from what I have seen in the past. I have never seen it work any other way. The software must know where center is in order to make the calcs.

 

The backplot may have looked wrong in X3 due to the origin issue.

 

Please let me know if you need any other help. I can run your code through Predator here if that's what it takes. My guess is that this will fix you up though.

 

 

Mike

[Mick]

Mike,

 

Thanks for the reply, and for looking at the file.

 

We tried setting it to the centre of rotation, but Vericut still didn't produce the correct results.

 

Interestingly, X2 didn't "flip" the part or axes, when backplotting, but did when opening the part in X3.

 

We couldn't get it to run, and since time was pressing, we generated a 3 axis path for it, using a side and face cutter. I would have liked to have gotten the 4 axis toolpath working, but we just plain ran out of time.

 

I will probably revisit this when I have some time.

 

Thanks again.