[platonas1]

Hello all.

I am trying to machine a part using 5-axis ( cms berbana ) machine and facing some problems. Simple part to machine a 45 degrees chamfer.
This is my first time programing in 5 axis.
Until now I place the part on the cnc table and take the dimensions of X/Y/Z using engraving tool. Then import them in machine offset G55.
On mastercam I just have to place the origin on top left corner, (same as g55).all is good when working.
Now I did the same for the part on the cnc, and in mastercam I used new plane to machine the chamfer I want.
The machine is turning the head 45 degrees but in wrong direction, and also moves to wrong place of the part.

Any help please?

[Superman]

It's not true 5 axis programming.... but 3+2 axis positioning


WCS is the view when the machine is all at zero ( .... your actual setup )
T/C planes is the view at which the machining is done.....AND that view must be obtainable ( using the table rotations ) from your WCS setup

so.... in the operation..... WCS is set to "TOP" .... both T&C planes set to "Plane"
"TOP" & "Plane" must have the same origin point (0,0,0)
What this does is let Mastercam work out the rotations needed to get to the other view

Does your machine have TPC ( tool path control ) ?.... or some sort of origin shift macro for multi-axis work ?
---- or do you have to set the new plane to another co-ordinate system ?

[platonas1]

I wish I can answere that.
I thought it would be easy using the +2 axis just
Changing the planed in mastercam.

I have no problem machine without rotate head.

I use fanuc 5 axis head vertical post processor from mastercam.

Maybe this is the problem?

It's not true 5 axis programming.... but 3+2 axis positioning


WCS is the view when the machine is all at zero ( .... your actual setup )
T/C planes is the view at which the machining is done.....AND that view must be obtainable ( using the table rotations ) from your WCS setup

so.... in the operation..... WCS is set to "TOP" .... both T&C planes set to "Plane"
"TOP" & "Plane" must have the same origin point (0,0,0)
What this does is let Mastercam work out the rotations needed to get to the other view

Does your machine have TPC ( tool path control ) ?.... or some sort of origin shift macro for multi-axis work ?
---- or do you have to set the new plane to another co-ordinate system ?

[warrenb]

Check the normals of your planes.

[platonas1]

Ok I hope you can find more details on my problem and maybe you can help me.
I made two videos.


1st) video showing the programming of the part I want to machine.
2nd) video shows the wrong movement of the machine head.

Like I said, I have no problem machining a part from top, the procedure is the same,
In mastercam origin is bottom right corner (top of part) and in the machine using a tool
I take the coordinates from part (bottom right) in place them into g55 machines work offset.

Thank you for your time taking to view these videos.


1st Video

[platonas1]

2nd Video

[Superman]

Your setting of the "Plane" is incorrect

for TOP view the gonom for the X+ direction is to the right
- when you set the bevel the X+ direction is aligned to the Y+ (TOP)

B is rotation around Y.... so the Y+ direction would not alter when just your head rotates to -45°
( when you create the new plane, the gonom should just do that -45° rotation.... the X+ should still point to the right, Z+ always point back up the spindle )

in your #1 video ( 30 seconds mark), the dialog has L/R arrows to toggle through other planes available to set that face ( some may have Z going back through the part, so.... this is the point that is critical, and where you need to re-create another plane )
( in the operation you need to re-select that new plane & regenerate ).

[Superman]

Hello superman,

thanks for your help?
Can you help me a little bit more please?
because i didnt undestand, I 've tried changing the planes with x direction to the right nut still have problems.

what is the right setup?

thanks in advance

Putting your PM into the thread for all... ( it can be difficult to comprehend, at the best of times )
but I think you use the correct WCS..... but defined the R/H bevel incorrectly

The relationship between the "New Plane" to your setup is...
- the WCS is the way your part is set on the machine ( when viewing from TOP ), your graphic Mastercam origin is where you set the part(work) origin in the machine
----- when doing 3+1, 3+2 or 5 axis work.... ( when programming, it is the TOOL that does the moving around your part... the part is always stationary )..... that WCS is the one that is set in the toolpath operations ( for the operations done in that setup)
----- the Tool & Construction plane is the one that tells the machine the angles FROM the WCS that the head has to move to ( unless you use a tool that alters the spindle axis..... T & C planes will always be the same )

---- WCS is set to "Your Setup -TOP", the T & C planes are set to "New Plane" ....... the origin for both views should be the same 3D reference point.......these need to be set in the toolpath operation..... for the op to create the correct path, WCS & the T/C plane need to be set before that operation is created.
NOTE..... Does your machine have TPC ( Tool Point Control ) ?....... this allows the current part origin to be maintained at the WCS position while using any B &/or C rotation.
Otherwise you need to set a separate coordinate at each & every plane you create IE G54 is origin of TOP, G55 for right bevel... etc, etc. ..... a real pain if you have lots of planes

( to get different work offset numbers (post must read the work offset areas) ,,,, in the plane manager for each view a -1 defaults to a G54 output...0(zero) outputs G54, 1=G55, 2=G56 etc )

a good way to check your view, is to set that new plane active then view it from TOP..... is it the view as seen by the head ?
ie the rear bevel

For a horizontal machine... the WCS is the TOP view.... T & C for B0° is FRONT view...... then RIGHT would be B90°, BACK =B180° & the LEFT=B270° fall into place automatically( or any other angle of that axis) ......
( if you use T&C=TOP, B0 is output, but any other views are NOT correct [ they're rotated sideways ].

It may be that your CNC_Machine ( in Mastercam) is not defined correctly, or your post modified ( is it a 5 axis post ?), or your machine is not yet fully understood in what info is required for a different programming method
- it is a bit of trail & error...... you need to experiment with what WCS & plane views combination gives the correct result...... I put up the Horizontal info to highlight a different train of thought may be needed

[warrenb]

The C or the B is reversed. In your code change the C to -90 or the B to +45 and see what happens.

Ok I hope you can find more details on my problem and maybe you can help me.
I made two videos.


1st) video showing the programming of the part I want to machine.
2nd) video shows the wrong movement of the machine head.

Like I said, I have no problem machining a part from top, the procedure is the same,
In mastercam origin is bottom right corner (top of part) and in the machine using a tool
I take the coordinates from part (bottom right) in place them into g55 machines work offset.

Thank you for your time taking to view these videos.


1st Video

[platonas1]

Yes the machine have TCP ( FANUC 18i mb ) How I can use it?

Is this G43.4 In my post?

:0001(TESTAXES)
(DATE=DD-MM-YY - 14-12-16 TIME=HH:MM - 18:23)
(MCX FILE - C:\USERS\PLATON\DESKTOP\TESTAXES.MCX-9)
(NC FILE - C:\USERS\PLATON\DESKTOP\TESTAXES.NC)
(MATERIAL - ALUMINUM MM - 2024)
(T17|50 FLAT ENDMILL |H17)
G21
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(50 FLAT ENDMILL |TOOL - 17|DIA. OFF. - 17|LEN. - 17|TOOL DIA. - 50.)
T17 M6
G0 G55 G90 X-21.163 Y-455. C90. B-45. S7000 M3
G43.4 H17 Z28.787
Z-11.213
G1 Z-21.213 F1300.
Y30. F8000.
G2 X-14.109 Y37.054 I7.054
X-7.054 Y30. J-7.054
G1 Y-430.
......
....