Multiaxis cutter compensation

[AlbertZini]

How to enable in Mpmaster postprocessor - cutter compensation in multiaxis ("4 axis") strategy ?

[AlbertZini]

If I turn on the tool compensation - "COMPUTER" "CONTROL COMP" "WEAR COMP" "REVERSE WEAR COMP"

is not that the program is not changed

 

 

 

 

(T219 - 10. FLAT ENDMILL - H219 - D219 - D10.000mm)

G00 G17 G21 G40 G80 G90

G91 G28 Z0.

(COMPENSATION TYPE - WEAR COMP)

T219 M06 (10. FLAT ENDMILL)

G00 G17 G90 G54 A0. X22. Y0. S1909 M03

G43 H219 Z120.

Z30.

G94 G01 Z20. F190.9

X15. ---------------- G41 D219 X15. F381.8(need cutter compensation)

A4.091 F1093.8

A8.182

A12.273

A16.364

A20.455

A24.545

...........

...........

...........

A-40.909

A-36.818

A-32.727

A-28.636

A-24.545

A-20.455

A-16.364

A-12.273

A-8.182

A-4.091

A0.

X22. ---------- G40 X22. (need cutter compensation)

G00 Z30.

Z120.

M05

G91 G28 Z0.

G28 Y0.

G90

M30

%

 

Please how to implement it !!!

[Elvincnc]

How to enable in Mpmaster postprocessor - cutter compensation in multiaxis ("4 axis") strategy ?

Actual theme,maybe mastercam does not have it or nobody does not know how to do it.......

[Guest]

It's not in there because "most" controls don't accept cutter compensation on 4 and 5 axis paths

[EX-wccprogrammer]

This can be done entirely in the post. You just need to make the post understand when to activate the comp and when to turn it off. The NCI file needs to be analyzed for data that could be accessed for a trigger. Also take a look at the available parametric values for the specific toolpath that you are using, there may be something that is normally unused that could be hijacked. Or you could opt to use a miscellaneous integer as a switch.

[AlbertZini]

If I understand correctly is responsible for this procedure "pccdia"

and for compensation for tool in my case "15346-2 compensation type = 2 wear". "15347-0 compensation direction. 0 = left"

But I do not understand how to write correctly in the post, and why compensation is disabled when the multi-axis is enabled

[EX-wccprogrammer]

A standard post will probably disable cutter compensation when multi-axis is enabled because most machines do not allow compensation in multi-axis. In multi-axis mode, compensation becomes a 3-axis (or more) adjustment and is way more complicated.

Machine controls track the centerline of the tool and can apply compensation relative to the toolpath. But they do not track actual angle of engagement of the tool, making it difficult (if not impossible) for the machine to apply compensation effectively in multi-axis.

[AlbertZini]

Thanks for the reply EX-wccprogrammer now I understand you.

When a lot of parts with little tolerance 10-0.02 mm we must regenerate a program that would go to that value or compensation to write by hand

[NCDataServices]

Hello

 

2D cutter compensation applies only to the diameter (radius/2) of the cutting tool in a plane that is normal (perpendicular) to the tool spindle (ie. XY plane). The information needed to do this is tool relation to the part in direction of cut; LEFT (G41) or RIGHT (G42) or OFF (G40). The amount of compensation is provided at the CNC usually in the D register and can be adjusted at the CNC.

 

It should be noted that a linear move (G1) with both X & Y should be programmed with the cutter compensation block. This move should also be at least as long as the value antisipated in the D register.

 

2D compensation D register value can represent the full tool diameter, radius or only the difference (trim) between the programmed and the actual tool radius. The program point needs to be the tool contact point for full diameter or radius compensation or the program point needs to be the cutter center point for difference (trim) compensation.

 

Many CNC have refered to 3D compensation but it is really only the same 2D compensation in any plane (not just XY plane). On rotary head muli-axis machines this can be done using G17, G18 and G19 for planes parallel to the machine co-ordinate axis. When planes are not parallel to the machine co-ordinate system a local co-ordinate system can be setup and used with the CNC (G68).

 

Multi-axis (5-axis) machines where the part rotates to bring the part in position to orient the tool axis vector parallel to the machine (tool) spindle has always been able to do 2D compensation in any plane because the tool spindle is fixed in the machines XY plane.

 

True 3D compensaion is required for radius compensation on a 3D surface machining. This can be a requirement in both 3-axis and 5-axis machining. True 3D compensation applies to the tip of the tool and is usually applied to ball end mills. The information required is a surface normal vector supplied by the CAM system at each tool position point (APT GOTO point). This surface normal vector (UVW) is independent of the tool axis vector (I,J,K) and the tool position (XYZ) can be the tip of the ball end mill (XYZ)or more common the center of the ball end mill (XYZ). The actual contact point with the surface is typically not required.

 

The compensation is computed by creating an offset surface by the (constant) distance of the compensation along each surface normal vector. This offset surface is not a linear translation because the curvature is not the same as that of the actual part surface. If the offset surface is away from a concave part surface the radius of curvature will be smaller. If the offset surface is away from a convex part surface the radius of curvature will be larger. This is an easy computation:

 

OffsetX = CenterX + (SurfaceNormalU * CompDistance)

OffsetY = CenterY + (SurfaceNormalV * CompDistance)

OffsetZ = CenterZ + (SurfaceNormalW * CompDistance)

 

Where:

OffsetX, OffsetY & OffsetZ are the compensated tool path points (XYZ)

CenterX, CenterY & CenterZ are the programmed center of the ball end mill (XYZ)

CompDistance is the compensation distance constant

SurfaceNormalU, SurfaceNormalV & SurfaceNormalW are the surface normal vector components (U,V,W)

Note that the U.V,W must be the signed components of a unit vector (1.0 unit long)

 

NC4EVER,

NCData

 

 

[AlbertZini]

I understand what you mean,i want to use cutter compensation only 4 axis , when there is a milling left or right side of mill

[djstedman]

This wouldnt solve your initial question for how to do this in a post.. but just a thought.. maybe if it is only x values you could use macro variables for the given positions in X and have them set at the beginning of the program.. then you effectively make your own comp in the X axis without ever actually turning comp on.. Just a thought and might not work for your situation.. just figured I would throw the idea out there in case it helped you..