# Thread: What am I doing wrong here with 4th rotary toolpath!

1. ## What am I doing wrong here with 4th rotary toolpath!

Mastercam X.

What I have done is open a new MC window.
Select everything = to left plane
draw a 1x1 box on the left plane
then contour, single and select just the top line of the box
then go into WCS, select T and C for the front veiw
then I select contour, single then select the front line.
I do this for the bottom and the back.

When I go to post, there is a A0, then A-90, then A-180 but no 270 degree.

I am selecting Axis positioning, x axis as for an A Axis.

Any Ideas?

2. If you are programming for a vertical machine
then the BACK & BOTTOM views are incorrect--- they are drafting views & are not capable of being achieved on a machine with the 4th axis around X.

- they should be created as seen by the operator ( or by the tool looking in the Z- direction ) as it rotates around the axis.

Your WCS for all operations should be TOP. ( this is your actual setup, & angles all relate back to this view )

your T/C planes you should use :-
- TOP view gives the A0. output
- FRONT view would generate the A-90.
- NEW BOTTOM ( rotated around Z by 180° ) gives A180. or A-180. ( depends on what direction you come from )
- NEW BACK ( rotated around Z by 180° ) gives you the A90. ( or A-270. )

Horizontals
- WCS is TOP for all ops, working face is FRONT ( gives B0. outputs )
RIGHT(B90.), BACK(B180.) & LEFT(B270.) all fall in correctly.

TOP & BOTTOM views are NOT usable on a 4-axis horizontal

3. So Let me think through this. The top veiw is just like if a part were in a vice on a regular vertical mill. The bottom view is 180 from that. I am not understanding why on a fourth axis, A axis, you cannot rotate the part 180 degrees to get the bottom view.

4. Work around. Assign 4 Work Offsets (0-Top, 1-Back, 2-Bottom, 3-Front=G54, G55, G56, G57). Program each Operation with appropriate WCS and Force Tool Change. Output will show all A0. Instruct operator to input G54 A0., G55 A90., G56 A180, G57 A270. in machine's work offsets.

• So you have to setup a new work offset for each rotary path?

Would if you had a part with 30 sides to it? There arent 30 offsets on most machines.

• This is what it is posting

N100 G20
N102 G0 G17 G40 G49 G80 G90
/ N104 G91 G28 Z0.
/ N106 G28 X0. Y0.
/ N108 G92 X10. Y10. Z10.
( 1 INCH FLAT ENDMILL TOOL - 1 DIA. OFF. - 0 LEN. - 1 DIA. - 1. )
N110 T1 M6
N112 G0 G90 X0. Y1. A0. S1000 M3
N114 G43 H1 Z1.1 M8
N116 G1 Z1. F10.
N118 Y-1.
N120 Z1.1
N122 G0 A90.
N124 Y1.
N126 G1 Z1.
N128 Y-1.
N130 Z1.1
N132 G0 A180.
N134 G1 Z1.
N136 Y1.
N138 Z1.1
N140 G0 Y-1.
N142 G1 Z1.
N144 Y1.
N146 Z1.1
N148 M5
N150 G91 G0 G28 Z0. M9
N152 G28 X0. Y0. A0.
N154 M30

• Originally Posted by blakemachine
So you have to setup a new work offset for each rotary path?

Would if you had a part with 30 sides to it? There arent 30 offsets on most machines.
A part with 30 sides to it, eh? I think you have shown me I have no reason to continue to assist on this matter. Good luck.

• I am not trying to be rude or anything. Sorry if it came off that way. I am just trying to learn this part of the software. Where if you had a part with flats every ten degrees or something. Can the software just run a A move after each milling opperation, to acheive this without using new work offsets?

• Use the transform toolpath as shown in the piture

PS what version of MC-X are you running I did this in X4

• Originally Posted by blakemachine
So Let me think through this. The top veiw is just like if a part were in a vice on a regular vertical mill. The bottom view is 180 from that. I am not understanding why on a fourth axis, A axis, you cannot rotate the part 180 degrees to get the bottom view.
You are correct in the way you are thinking....but that BOTTOM view is NOT how the tool sees your part on the CNC machine. You should be using views that the machine is capable of achieving in that setup, ie you can't use the RIGHT SIDE can you, but you could program operations on that face...yes ?? ---all the NC code would be wrong, X&Y values swapped around, a real mess

Say you had a vice sitting in space ( with the tightening screw pointing in the X- direction ) ( in Mastercam )

now if you select the standard views
TOP view is correct, screw points to left, vice base is below part
FRONT view is correct, screw points to left, vice base is at the bottom of screen
but for the
BACK view, screw points to right, base is at bottom of screen
BOTTOM view,screw points to right, base is above part

both these views have to be individually rotated around Z by 180°, ( & then named), so that those screws all point in the same direction ( & to use only 1 co-ordinate system (G54) they all must have the same origin point, which must lie on the axis of rotation )

Check what WCS you have for that rear operation ( it should be TOP), as well as what T&C plane you used ( it should be BACK-ROTATED 180° )