5 axis question - HMC machine

[c0penhague]

hi all...

 

Im completely puzzled over here... imagine running a rotary table that is seating off the center of the main center of rotation on a HMC...

the post was changed with the appropriate values to compensate the shift, on the mastercam the part is programmed according to the views [right view]... front plane is B0. C0. ...

The G-Code outputs pretty good except the Z value... because G54 Z value is taken from the exact main center of rotation the G-code Z values are very difficult to measure but seemed okay...

 

Is there any way of programming it that the Z value would come out as a normal 3 axis machine?

 

thank you all

[K2csq7]

Move the orgin of your toolplane to where you want your Z zero to be.

[gcode]

This is a 3+2 double rotatary setup...using a standard Generic Fanuc 5X post

 

I do it like this

 

 

#Axis shift

shft_misc_r : 0 #Read the axis shifts from the misc. reals <---------------Make sure this value is 0

#Part programmed where machine zero location is WCS origin-

#Applied to spindle direction, independent of RA

#Table/Table -

#Offset of tables to secondary axis relative to machine base.

#Tilt Head/Table - Head/Head -

#Part programmed at machine zero location-

#Offset in head based on secondary axis relative to machine base.

#Normally use the tool length for the offset in the tool direction

saxisx : 0 #The axis offset direction?

saxisy : 0 #The axis offset direction?

saxisz : 0 #The axis offset direction? ***** Set Z to B C/L distance here ****** <-------- Set your pivot distance here

# distance is absolute from Mastercam file origin

# if part is in front of B C/L "saxisz" will be a negative number

# Note.. Z tool length offsets will be set from Mastercam Z0 not

# center of B axis*******

 

 

Z values for 3 axis toolpaths will look just like a 3X mill program

5 axis values are comped from Mastercam Zero as it rotates about the pivot point.

This makes nice code because its easy for the oprator to read and understand 3X toolpaths.

 

You can also do this by setting

shft_misc_r to 1

and using mr 7 8 and 9 in each operation to define the pivot point

 

# mr7 - Axis shift for X axis, See 'shft_misc_r'

#

# mr8 - Axis shift for Y axis, See 'shft_misc_r'

#

# mr9 - Axis shift for Z axis, See 'shft_misc_r'

 

I don't like to do it this way because if you forget to set one or 2 cuts in the middle

of a 300 op file, you're going to get a very ugly crash..

 

 

 

 

 

[c0penhague]

well... thanks guys..

in regards to the tplanes- it might work indeed, just have to figure out how to....

 

the post heh? I don't feel like playing around... this project is very critical- there is no margin to mistake, but thanks...

 

 

do you guys know anything about this theory below?

 

G54

It also states to place the model/part or stock in respect of the machine origin......

(or another way to look at it ).....

program it around the "normal views" , create another WCS with the origin at the machines' rotation origin

( HINT, place a point to represent the rotating origin and use this point when setting the XYZ origin in your WCS and T/C planes.... moving this point would move your toolpaths as well.

It is also a good idea to keep the standard views untouched, create your own WCS and views and adjust the origin on these, )

[K2csq7]

well... thanks guys..

in regards to the tplanes- it might work indeed, just have to figure out how to....

 

Easiest for me is to create 2 lines that intersect where you want the orgin to be, one vertical representing Y+, and one horizontal representing X+. Then click planes at the bottom, planes by geometry, pick your X line first, then the Y line. Make sure the gnome that pops up looks correct (it will let you cycle through a few choices, but if you do exactly as I stated the first choice it gives you should be the correct one.)

 

 

 

 

[c0penhague]

Easiest for me is to create 2 lines that intersect where you want the orgin to be, one vertical representing Y+, and one horizontal representing X+. Then click planes at the bottom, planes by geometry, pick your X line first, then the Y line. Make sure the gnome that pops up looks correct (it will let you cycle through a few choices, but if you do exactly as I stated the first choice it gives you should be the correct one.)

 

I will try that indeed.

have a great day and thankx...

[John Morris]

cOpenhague,

 

Which post did you start with to get this setup to work? I have the same situation here. I have a Haas horizontal with the 5 axis option so the additional 4th can be placed on the pallet and plugged in when needed. Did you start with the Generic Fanuc 5 axis post that Gcode mentioned or something else? I need to start working on one for myself and am looking for input on the best base post to start from so I don’t get half way through and wish I had started with something else.