Rotary Axis (A) On Vertical Mill - Bug?

[Mick]

Ok, I was just trying something

 

I'm programming a part on a rotary axis. Okuma MB56 Vertical with A axis. I'm drilling a hole through a flat surface that is at A0, but sits below the axis of rotation (imagine like a trunnion table, and the flat surface of the table is below the centerline of the A axis).

 

Using toolplane Top (A0) it drills the part from the underside, and when posted, outputs A180 (which is incorrect). If I translate the hole above the centre of rotation, it drills correctly (from the top) and outputs A0 (correctly).

 

This is using Rotary Axis postioning, as I want to output the A command.

 

Now, maybe I'm using this wrong, but from what I can see, I'm not. The interesting thing is, that with the hole positioned below the centre of rotation, and then using Toolplane Bottom, it outputs A180 and positions the tool correctly. As a fix, I can translate the hole geometry above the axis of rotation, but surely it should stay in top plane regardless of what z depth the geometry is positioned at?

 

If I'm missing something, please throw me a peanut...

[gcode]

are you using a regular 2D toolpath or a 5 axos toolpath.

a 2D toolpath woithout rotary positioning should give you a good canned cycle, but won't output the "A"

I'd try a 5X toolpath with point/line driving geometry

[Mick]

I'm using 2D drilling (not multi axis), and rotary axis positioning under Rotary Axis Control should output the A.

[gcode]

if you're doing 2D toolpaths on multiple faces, defined by toolplanes, you don't need to use Rotary axis control.. thetoolplanes will force

athe A output.

 

the problem is forrcing the rotary output if your just using Top toolplane... that's why I suggested

5X drilling .. maybe it willforce the A output

[Mick]

Ok, I understand what you mean. 5 Axis will output the necessary A moves. And that it does

 

My point is, to ensure A0 is output, without resorting to a 5 Axis toolpath, then using Rotary Axis control, with Rotary positioning should provide the correct A output.

 

Kind of like using a gas cutting torch to open a can of beans. 5 axis is like a gas cutting torch, and a good ol' tin opener is 2D with Rotary positioning

[Chris Rizzo]

random thought, try "combine arcs" and see what happens.

[Mick]

random thought, try "combine arcs" and see what happens.

 

Combine Arcs? Where is that?

[DavidB]

What are you using for the drill point geom an arc?

I don't think you should have to resort to 5-axis to do this job. Not everyone has the 5-axis add on.

 

Try using a point created at the centre of your arc below the centre line of the A axis.

[Mick]

I'm using arc center points, and I agree, it's a 2d drilling operation, and shouldn't need the multi axis addon

[gcode]

The only time this is an issue is if you're doing 1 operation in top plane..

you won't get the A output. if you're doing work on multiple toolplanes, the post will see the

rotation and output the "A"s without using the Rotary axis switch.

There is a simple post tweak to force the A, but I don't recall what it is.

Are you using anmpfam post or mpmaster?

 

 

[gcode]

If you're running mpmaster, try playing with this switch

 

rot_on_x = 0 #Turn off rotary axis unless it is detected in machine read - supresses rotary output in 3 axis machines

[Guest]

Mick,

 

Have you tried Screen >> Combine views?

 

Not knowing your geometry it's possible it's drawing in a different view?

[Alex_AMEAB]

This is my solution:

 

pfcout
    #if index = zero & rot_on_x
     #[
       if use_rotmcode & (fmtrnd(cabs) <> fmtrnd(prv_cabs) | sof), *sindx_mc
       if absinc$ = zero, *cabs, !cinc, !cout_i
       else, *cout_i, !cinc, !cabs
     #]

 

It looks like rot_on_x is set to 0 first time the post enters the ptlch_com section. Therefore no A0 output.

Doing this will move the output of A to the G00 G90 G54 yada yada line (uless you move it in the post ofc).

Seems to have no effect on the output when doing simultanious 4axis toolpaths

 

edit: This is from mpmaster

[Mick]

Ok, I've attached two MCX-6 files to demonstrate the differences.

 

The Above Zero file outputs the A index correctly, and the Below Zero doesnt. Note that both use the top tool plane, and both holes are in the same plane, just in different Z positions.

 

Below is the posted code. The T.MIN file is for the Above Zero, and the T2 is for Below Zero.

 

The post I am using is MPMaster Okuma post.

 

The point is, I want to force the A output, even for single operation posting. And the post is working correctly, as it is posting out what I see in Mastercam

 

Here are the two posted programmes:

 

Above Zero: (Correct Output)

 

$T.MIN%

(T)

(DESCRIPTION:

(MACHINE: OKUMA MB56VA/E100M CONTROL)

(DATE/TIME: 19-06-12/08:23)

(WORKPIECE ORIGIN:

(WORKPIECE ORIENTATION:

(TOOLS:)

(T1 - 16MM UDRILL - D16.00mm)

 

G15 H1

 

NAT1 (U-DRILL 16MM HOLE)

S6000 M3

G0 G17 X100. Y0. A0. M15

G56 Z55. H1 M8

G81 Z30. R55. F300. M54

G0

G80

Z900. M5 M9

X-300. Y900. A0.

M2

%

 

Below Zero: (Incorrect Output/Toolpath Wrong)

 

$T2.MIN%

(T2)

(DESCRIPTION:

(MACHINE: OKUMA MB56VA/E100M CONTROL)

(DATE/TIME: 19-06-12/08:23)

(WORKPIECE ORIGIN:

(WORKPIECE ORIENTATION:

(TOOLS:)

(T1 - 16MM UDRILL - D16.00mm)

 

G15 H1

 

NAT1 (U-DRILL 16MM HOLE)

S6000 M3

G0 G17 X100. Y0. A180. M15

G56 Z10. H1 M8

G81 Z-15. R10. F300. M54

G0

G80

Z900. M5 M9

X-300. Y900. A0.

M2

%

ROTARY AXIS - ABOVE Z0.MCX-6

ROTARY AXIS - BELOW Z0.MCX-6

[Jayson Kramer]

Mike check your mail and post.

[Mick]

Ok, so Jay has made it work

 

Weird though, as to make it work, he had to set the rotary axis to rotate about Z. But, this is an A axis (therefore rotating about X)

 

Me = confused

 

But, I just have to say, I love this place. Where else can you get this kind of assistance?

[Jayson Kramer]

This is not the right way and these Axis sub paths are not made for what you are doing. really need to follow what the rest have stated of the option for paths.